-->(Par_cf)-->|center|--->|focus|---->
-->(Par_fdp)-->|focus|-->|direction|-->|end pnt|---->
With Par_cf you indicate the center of the parabola, and then the focus of the parabola.
With Par_fdp, you indicate the focus of the parabola, then the direction of the parabola, and then the end of the parabola.
-->|letter|---+--------------+--->
| |
+---|letter|---+
| |
+---|digit|----+
| |
+----(_)-------+
This describes the syntax of a parameter name. A parameter name follows the same restrictions and guidelines as macro names. Parameter names must not conflict with existing command names, qualifiers, macros, etc.
Parametric Design adds full parametric modeling and constraint-based capabilities to ME10. Any existing ME10 drawing can be used with Parametric Design.
Parametric modeling lets you assign 'names' or parameters to drawing dimensions, such as radii or lengths, and then modify the drawing by changing the numerical values or expressions associated with these parameters.
Constraint-based modeling lets you specify geometric properties and relationships. The software then modifies the part so that these constraints are satisfied. For example, you can say "these two elements should be tangent", or "this line should be horizontal", or "this dimension should have such-and-such a value". Constraints can be assigned explicitly or they can be generated with Design Intent Capture.
Parametric and constraint information is converted to INFO text when the part is stored and converted back to the internal format when the MI file is loaded.
With Parametric Design, a 'master' part can be created and variations can be generated quickly by changing parameter values. The combination of parameters and constraints provides an alternative to the MODIFY menu for drawing modification.
,-----------------------,
v ^
--+--'/'--+-->|simple name|--+--'/'-->|simple name|--+-->
v ^ v ^
'-------' '-----------------------'
A part name is a series of one or more simple names separated by slashes, and possibly beginning with a slash. A simple name can contain any character except slash.
Each part has a simple name. If this simple name is unique, then the name can be used to identify the part, and no slashes are needed, regardless of where the active part is. Simple names need not be unique, however, so the slash notation is used to give each part an unambiguous name. The naming scheme is very much like the UNIX-based file tree. 'abc' names a part in the active part. '/' names the top-level part (root). 'abc/def' names the part def in the part abc in the active part. '/abc/def' is similar, except 'abc' is found in the top part instead of the current directory.
Within a part name, the double period (..) refers to the parent of the part named so far, and the single period (.) refers to the part itself. If these constructs appear at the beginning of a part name, the active part is considered the "part named so far". Thus, the single period (.) is a way of naming the active part without having to remember its real name, ../xxx names a part xxx which is a sibling of the active part, and so on. If the part named so far is the top, then the double period (..) is the same as the single period (.).
Currently no checks are made to ensure that parts have unique names within a given directory. Furthermore, when a part is copied, the copy has exactly the same name as the old part. Thus, it is possible that a part has no unambiguous name, and so must be identified in some other way (for example, by picking an element belonging to it).
This section is a brief introduction to parts. For help with specific parts commands, enter HELP with the command name, or say HELP PARTS and then use the N (Next) command of the help system.
A part is an element that contains other elements. Thus parts group elements together. Don't take the name "part" too literally. The elements grouped into a part needn't have any physical meaning; they are simply grouped for the purposes of the drawing.
Parts impose a hierarchy on the elements of a drawing. At the top of the hierarchy is a part named (initially) "Top". The top part is the only element that does not belong to a part. It is present in every drawing, even before you add any elements, and cannot be deleted.
Except for the top part, all elements belong to exactly one part. A part belonging to another is known as its "child"; similarly, a part containing another is its "parent". Unlike human families, a part child never has more (or less) than one parent.
One (and only one) part in the hierarchy is called the "active part". The name of this part is shown in the status line. EDIT_PART lets you choose which part is active. The active part is the part in which all new elements are automatically placed. Furthermore, you can only delete or modify elements in the active part. (There are a very few exceptions to these two rules: CREATE_DETAIL and LOAD can both produce elements in other parts, and GATHER can remove elements from other parts.)
There are two ways to make a new part. You can create the geometry, then impose a parts structure on it, or you can create the parts first, then fill them with geometry. CREATE_SUBPART is the command for the first method. INIT_PART and INIT_SUBPART are the commands for the second.
Once you have a parts structure, GATHER allows you to move elements from one part to another.
SMASH_SUBPART deletes a part but retains its elements.
Except for the commands already mentioned, which are all commands that change the parts structure, there are few special commands for manipulating parts. The reason is simple: parts are elements, just as, say, lines are, and can be manipulated with the same commands as other elements. To delete a line, for example, you say DELETE, then identify the line. To delete a part, you say DELETE and identify the part. You identify the part by digitizing any geometry in it.
The fact that parts have several layers of structure introduces some complexity into the process of identifying elements. The problem is that (unless you use SHOW_PART) there is nothing on the screen that corresponds to a part itself; you see only the geometry that it contains. Thus, without some convention imposed by the system, there would be no way to unambiguously identify a part with the tablet or mouse. (You can always enter the name of the part, but this is often less convenient). If you digitize a line, for example, and you are in the DELETE command, do you want to delete the line, or the part containing it, or that part's parent, or ...?
To make the identification unambiguous, we use the parts structure itself to impose the following convention. We assume that you always want elements in the active part. Thus, if a line is contained in part A, and part A is in the active part, and you say DELETE and identify the line, then we assume you want to delete part A. Part A is, at this level, a single entity that cannot be treated as individual elements. Of course, you can always make part A the active part; then the members of part A can be manipulated individually. This is the reason for the rule, mentioned above, that you can only delete or modify parts in the active part.
Unfortunately, this identification convention is not completely consistent throughout the system. Sometimes the convention would make little sense. Consider EDIT_PART, for example. We want to use EDIT_PART to edit a part on the screen. We would like to digitize the new part. It would be a serious limitation to require that we could only identify parts in the active part. Therefore, EDIT_PART has its own rules about how parts are identified, rules that allow you to identify parts anywhere in the parts tree. There are other commands that do not follow the "only in active part" convention, but they all, like EDIT_PART, are ones that do not change your drawing data. Commands that change your data (modify, delete, change text parameters, convert splines, etc.) are in general limited to the active part only.
A complex drawing may be drawn using several "parts" which may be considered as sub-drawings, each part may exist more than once in the overall drawing. This menu allows the user to create, edit, rename, smash, share and list the various parts which are contained in the drawing.
Some of these commands are duplicated on the tablet at the top right corner.
-->(PARTS_LIST)--+------------------+--+----------------(SCREEN)-----------+-->
v ^ | |
+-->(ALL)----------+ '--+-----------+--|file specifier|--'
| | | |
+-->(COUNT_TREE)---+ +-(DEL_OLD)-+
| | | |
+-->(TREE)---------+ '-(APPEND)--'
| |
'-->(LTAB)->|name|-'
PARTS_LIST shows the parts in the active part whose names do not begin with '.', along with a count of how many times each part occurs.
With the COUNT_TREE option, PARTS_LIST shows the parts subtree of the active part whose names do not begin with '.' including the active part itself, along with a count of how many times each part occurs.
With the TREE option, all parts are listed; the indentation shows the part structure. An asterisk (*) shows which part is active. The drawing scale of each part is also listed. Symbols and isometric views are labeled as such, and the shared parts are numbered.
With the ALL option, the ME30 system parts are also shown.
SCREEN sends the output to the built-in editor (see EDITOR). LTAB sends the output to a new logical table named 'name'. Otherwise, the output is sent to the file specified. With DEL_OLD, a file of the same name is overwritten without comment. With APPEND, the parts list goes at the end of the named file, if it exists; otherwise, a new one is created. With neither DEL_OLD nor APPEND, the presence of a file with the same name is an error.
You can get a parts list into the drawing as follows:
You now have a block text on your cursor, containing the parts list.
-->(PARTS_LIST_FORMAT)--+-->(STANDARD)-----+--->
| |
+-->(ENHANCED)-----+
PARTS_LIST_FORMAT defines the output format of the PARTS_LIST TREE function. The ENHANCED format of version 06.00 will be used by default.
STANDARD: this is the output format of version 05.xx. It should be used if
older macros depend on this special format. Information about
drawingscale or unique partname is not included.
ENHANCED: this is the output format of version 06.00. It contains additional
information about the new parts functionalities like drawingscale
and unique partnames.
+----<-----+
| |
--->(PART_DRW_SCALE)--+--|part|--+-->|scale factor|--+-->
| |
+--(ALL)---+
| |
+--(ONLY)--+
scale factor: number
PART_DRW_SCALE scales the geometry of parts and subparts with the specified factor (which is a number). This lets you have multiple drawing scales on one drawing. The scale associated with a part can be seen in the parts tree and on the status line. Text, dimensioning text, and symbols are not changed.
The option ALL scales the current part and subparts. The option ONLY scales the selected part only.
The center point for the scaling is defined by the current setting of the PART_DRW_SCALE_REF function and a yellow marker will show its position for the selected part.
--->(PART_DRW_SCALE_REF)--+-->(CENTER)-------+-->
| |
`---(PART_ORIGIN)--'
| |
`---(REF_PNT)------'
PART_DRW_SCALE_REF defines the scaling center for PART_DRW_SCALE, SMASH_SUBPART KEEP_DATA and GATHER KEEP_DATA.
CENTER is determined by the center of a box, surrounding all geometry
elements in the specified part. Scale invariant elements, like
symbols, texts and dimensiontexts are not included.
PART_ORIGIN is determined by the origin of the specified part.
REF_PNT is determined by the part reference point that can be set by the
SET REF PNT command in the PARTS menu.
Use this function to iconify/deiconify a parts tree. This function is useful when you have a large assembly and do not want to display nested parts.
-->(PART_NUMBER_OFFSET)--+--->(ON)----+--->
| |
'--->(OFF)---'
When a part is loaded as subpart, it will get a new unique part number. The function PART_NUMBER_OFFSET determines how this new unique part number is calculated. The default is OFF.
Option ON : The new part number will be
(highest part number in drawing + part number in MI file).
This can generate large gaps in the part numbering.
Option OFF: The new part number will be (highest part number in drawing + 1).
This is also the behaviour, when there are no unique part numbers
in the MI file.
-->(PASTE_FROM_CLIPBOARD)-->--+->-(NOSUBPART)->------------+-{position}-->
| |
+->-(SUBPART)--->-|partname|-+
The PASTE_FROM_CLIPBOARD function pastes selected items from either the ME10 native format (from other ME10 sessions) or the Enhanced Metafile Format (only from other Windows applications). Items can be pasted into the current part (NOSUBPART) or a new SUBPART can be created with the user's partname.
{position} depends on the format of the clipboard objects. If objects are text or me10 format, position is defined with one single point. If objects are in EMF format, position is defined with box.
CURRENT LIMITATION: When pasting plain-text on the viewport, pasting will ask user to enter the coordinates until 'end' has been passed. In this case, 'SUBPART' and 'NOSUBPART' have no sense. It is always pasted into the current part.
Use this function to highlight detail parts, symbol parts, or isometric parts.
-->(PD_AUTO_ANGLE_TOLERANCE)----|number|--->
This function specifies the absolute tolerance used during PD_RESOLVE AUTOMATIC constraint extraction to compare angles, such as checking whether two lines are parallel, or a single line is horizontal. The number supplied must be greater than or equal to zero. The initial value is 0.000001 radians.
-->(PD_AUTO_SAME_DISTANCE_TOLERANCE)----|number|--->
This function specifies the absolute tolerance used during PD_RESOLVE AUTOMATIC constraint extraction to compare two non-zero distances, such as checking whether two circular elements have the same radius. The number supplied must be greater than or equal to zero. The initial value is 0.000001 mm.
-->(PD_AUTO_SYMMETRY_COLOR)--+--|color|--+---->
| |
+---(ANY)---+
This function specifies the color of lines which will be treated as symmetry lines during automatic constraint generation. If ANY is specified then color will not be used to exclude lines from being automatically constrained as symmetry lines.
PD_AUTO_SYMMETRY_COLOR is used in combination with PD_AUTO_SYMMETRY_LINE and PD_AUTO_SYMMETRY_LINETYPE. The initial setting is ANY.
-->(PD_AUTO_SYMMETRY_LINE)--+---(NO)--+--->
| |
+--(YES)--+
This function specifies whether the automatic constraint generator should scan the drawing for symmetry lines. If so, then all lines which have the color specified by PD_AUTO_SYMMETRY_COLOR and linetype specified by PD_AUTO_SYMMETRY_LINETYPE will qualify. The initial setting is NO.
-->(PD_AUTO_SYMMETRY_LINETYPE)--+--|linetype|-----+--->
| |
+-----(ANY)-------+
This function specifies the linetype of lines which will be treated as symmetry lines during automatic constraint generation. If ANY is specified then linetype will not be used to exclude lines from being automatically constrained as symmetry lines.
PD_AUTO_SYMMETRY_LINETYPE is used in combination with PD_AUTO_SYMMETRY_LINE and PD_AUTO_SYMMETRY_COLOR. The initial setting is ANY.
-->(PD_AUTO_TANGENT_TOLERANCE)----|number|--->
This function specifies the absolute distance tolerance used during PD_RESOLVE AUTOMATIC constraint extraction to check whether two elements are tangent. One of the elements extracted must be circular. The tolerance is used to compare the radius of the circular element to the distance from the circular element center point to the other element. The number supplied must be greater than or equal to zero. The initial setting is 0.000001 mm.
-->(PD_AUTO_ZERO_DISTANCE_TOLERANCE)----|number|--->
This function specifies the absolute tolerance used during PD_RESOLVE AUTOMATIC constraint extraction to compare a distance to zero, such as detecting coincident points, collinear lines and point on element constraints. The number supplied must be greater than or equal to zero. The initial setting is 0.000001 mm.
-->(PD_DEFAULT_DIM_COLOR)--|color|-->
PD_DEFAULT_DIM_COLOR sets the display color of parametric dimensions drawn with PD_MAKE_DIMENSIONS.
-->(PD_DEFAULT_DIM_TEXT_SIZE)--|text size|-->
PD_DEFAULT_DIM_TEXT_SIZE sets the text height of parametric dimensions drawn with PD_MAKE_DIMENSIONS. The text size is given in the current length units.
+------------------------------------------------------------+
| |
| +----------------------------------+ |
v v ^ ^
-->(PD_FIX)-+-+-(PD_ANGLE_LINES)-+-|line 1|-|line 2|-+-----------+--+--+-+-->
| | | |
| +--|value|--+ |
| | | |
| +--|name|---+ |
| |
| |
| +-------------------+ |
| v ^ |
+-(PD_COLLINEAR)-+-|line 1|-|line 2|-+-------------------+
| |
| |
| +-----------------------------+ |
| v ^ |
+-(PD_DIMENSION)-+-|dimension|-+-----------+---+---------+
| | | |
| +--|value|--+ |
| | | |
| +--|name|---+ |
| |
| |
| +---------------------------------+ |
| v ^ |
+-(PD_DISTANCE)-+-|elm 1|-|elm 2|-+-----------+---+------+
| | | |
| +--|value|--+ |
| | | |
| +--|name|---+ |
| |
| |
| +-------+ |
| v ^ |
+-(PD_ELEM)-+-|elm|-+------------------------------------+
| |
| |
| +----------------------------------+ |
| v ^ |
+-(PD_FILLET)-+-|fillet|-|end elm 1|-|end elm 2|-+-------+
| |
| |
| +--------+ |
| v ^ |
+-(PD_HORIZONTAL)-+-|line|-+-----------------------------+
| |
| |
| +------------------+ |
| v ^ |
+-(PD_MIRROR)--|line|--+--|elm 1|-|elm 2|-+--------------+
| |
| |
| +--------------------------+ |
| v ^ |
+-(PD_POINT)-+-|point|--+-------------+-+----------------+
| | | |
| +---|name|----+ |
| |
| |
| +-----------------+ |
| v ^ |
+-(PD_POINT_ON)--+--|point|-|elm|--+---------------------+
| |
| |
| +-------------------+ |
| v ^ |
+-(PD_PARALLEL)-+-|line 1|-|line 2|-+--------------------+
| |
| |
| +-------------------+ |
| v ^ |
+-(PD_PERPENDICULAR)-+-|line 1|-|line 2|-+---------------+
| |
| |
| +---------------------------------+ |
| v ^ |
+-(PD_SAME_DISTANCE)-+-|elm 1|-|elm 2|-|elm 3|-|elm 4|-+-+
| |
| |
| +-----------------+ |
| v ^ |
+-(PD_SAME_SIZE)-+-|elm 1|-|elm 2|-+---------------------+
| |
| |
| +--------------------------+ |
| v ^ |
+-(PD_SIZE)-+-|elm|----+-----------+---+-----------------+
| | | |
| +--|value|--+ |
| | | |
| +--|name|---+ |
| |
| |
| +---------------------------+ |
| v ^ |
+-(PD_SLOPE)-+-|line|---+-----------+----+---------------+
| | | |
| +--|value|--+ |
| | | |
| +--|name|---+ |
| |
| |
| +----------+ |
| v ^ |
+-(PD_SYM_LINE)-+--|line|--+-----------------------------+
| |
| |
| +-----------------+ |
| v ^ |
+-(PD_TANGENT)-+-|elm 1|-|elm 2|-+-----------------------+
| |
| |
| +--------+ |
| v ^ |
+-(PD_VERTICAL)-+-|line|-+-------------------------------+
PD_FIX is used to define new constraints. These constraints will be used in future calls to PD_RESOLVE if the modify zone contains any of the elements involved. The meaning of each constraint type is described below in terms of how it effects PD_RESOLVE.
PD_ANGLE_LINES specifies the relative angle between two linear elements. If a value or name is not specified then the current angle is preserved.
PD_COLLINEAR will force two linear elements to be collinear.
PD_DIMENSION will cause the geometry associated with the dimension to take on the given value. If a value or name is not given, then the current value of the dimension will be preserved. If a parameter name is defined then either the value of the parameter will be used to define the geometry or the geometry will be used to define the value of the parameter.
PD_DISTANCE specifies the distance between any two point, linear or circular elements. If a value or name is not specified then the current distance is preserved.
PD_ELEM will maintain the position and size of the element.
PD_FILLET will force two real geometry elements to be filleted by a given circular arc. Each end of the arc must share an end point with one of the elements.
PD_HORIZONTAL will force a linear element to be horizontal.
PD_MIRROR will force the extension of two elements to be mirror images of each other about a given line.
PD_PARALLEL will force two linear elements to be parallel.
PD_PERPENDICULAR will force two linear elements to be perpendicular.
PD_SAME_DISTANCE will force the distances between two pairs of elements to be identical.
PD_SAME_SIZE will force two lines to have the same length or two circular elements to have the same radius.
PD_SIZE specifies the length of a line or the radius of a circular element. If a value or name is not specified then the current size is preserved.
PD_SLOPE specifies the slope of a linear element. The slope is measured counterclockwise relative to the positive x axis. If a value or name is not specified then the current slope will be preserved.
PD_SYM_LINE identifies a line as a symmetry line. Lines identified in this manner will be used by PD_RESOLVE GENERATE to search for pairs of mirrored elements.
PD_TANGENT will force two elements be tangent. One of the elements must be circular. Two elements can be tangent even if they do not touch. All that is required is that the extension of the elements are tangent.
PD_VERTICAL will force a linear element to be vertical.
+---------------------------------------------+
| |
-->(PD_FREE)-+-(NOBAN)-+-v-+-------------|id pnt|---------+-+--------+-^--+-->
| | | | | | |
+--(BAN)--+ | | +-(UNDO)-+ |
| | |
+--|kind|--+-+--(ALLTYPES)--+--+ |
| | | |
| +----|type|----+ |
| |
| |
| +----------+------------------------+ |
| | | | |
+--v--|type|--v--|select|--+--------+--^-------+
| | | |
| +-(UNDO)-+ |
| |
| |
+-------(ALLTYPES)---(CONFIRM)-----------------+
PD_FREE is used to delete one or more constraints.
Either BAN or NOBAN must be entered. If BAN is chosen then the constraints selected are marked deleted and prevented from being extracted by subsequent calls to PD_RESOLVE GENERATE. NOBAN removes the constraint from the database completely, meaning that it can be extracted by subsequent calls to PD_RESOLVE GENERATE.
The simplest method to remove a single constraint is to pick on the icon for the constraint. If a constraint is identifiable by two or more icons, then picking on any one of those icons is sufficient.
The second form of this command is used to free a subset of constraints. This subset is indicated by first selecting a constraint kind modifier and then selecting a constraint type or ALLTYPES. The kind modifier is BANNED, SYSTEM, UNUSED, USED, USER, VIOLATED. BANNED constraints are those which the user has explicitly banned with the PD_FREE BAN command. SYSTEM constraints are those constraints added by previous calls to PD_RESOLVE GENERATE and unmodified by the user. UNUSED are those constraints that were not used by the last call to PD_RESOLVE to determine the new geometry but were satisfied. USED are those constraints that were used in the last call to PD_RESOLVE to determine the new geometry. USER are those constraints added by the user or system constraints that were modified by the user. VIOLATED are those constraints that were violated by the last call to PD_RESOLVE.
The third form of this command parallels the PD_FIX command. Here the user identifies the constraint type to be freed and then selects the explicit geometry involved. All of the rules that apply to the selection of the geometry in PD_FIX also apply, with two notable exceptions. Since an arc can be a fillet in at most once way, it is sufficient to simply identify the fillet arc. And since an element can be mirrored to at most one other element about a given symmetry line, it is sufficient to identify the symmetry line and one member of the mirrored pair.
The final form of this command is used to remove all parametric information from the current part. This can significantly reduce the database and file size for storing the part.
Example:
PD_FREE NOBAN SYSTEM ALLTYPES
This is the simplest way to retain user defined constraints while removing all constraints generated by the system.
Example:
PD_FREE NOBAN ALLTYPES CONFIRM
This is the simplest way to free all parametric information from the part.
+-----------<-----------+
v ^
-->(PD_HIDE_DIMENSIONS)--+--|select dimensions|--+-->
PD_HIDE_DIMENSIONS removes selected parametric dimensions from the display. Parametric dimensions are displayed with PD_MAKE_DIMENSIONS.
+------------+
v ^
-->(PD_INFO_CONSTRAINT)--+--|id_pnt|--+----->
PD_INFO_CONSTRAINT is used to highlight the geometry associated with a constraint. The constraint is identified by picking its icon.
PD_INFO_CONSTRAINT is particularly useful for identifying quickly constrained pairs of elements (e.g. parallel lines, mirrored elements).
+------------+
v ^
-->(PD_INFO_ELEMENT)--+--|id_pnt|--+----->
PD_INFO_ELEMENT is used to query how PD_RESOLVE determined the position and size of the element identified by id_pnt during the last call to PD_RESOLVE in the current session. All constraints that were used in the determination will have their icons displayed and all geometry on which those constraints rely will have their geometry highlighted as well.
Using this command on an element which was not solved for in the last call will produce no icons or highlights.
If the constraints have been edited since the last call to PD_RESOLVE then the information returned could be misleading.
+--------<---------+
v ^
-->(PD_MAKE_DIMENSIONS)--+--|sel elements|--+-->
PD_MAKE_DIMENSIONS displays parametric dimensions associated with selected elements. Parametric dimensions are created when COPILOT is turned on. Parametric dimensions are removed from the display with PD_HIDE_DIMENSIONS.
+-------------<------------+
v ^
-->(PD_MODIFY_DIMENSION)--+--(IMMEDIATE)--+--+--|sel dim|--|new value|--+
| |
+--(DEFER)------+
PD_MODIFY_DIMENSION sets a new value for a parametric dimension. Parametric dimensions are created when COPILOT is on, and they are displayed with PD_MAKE_DIMENSIONS.
IMMEDIATE indicates that all geometry should be updated as soon as the new value is entered.
DEFER indicates that the value of the parametric dimension should be changed, but the geometry should not be updated until later. In other words, DEFER allows several parametric dimensions to be modified at one time. Performance is improved, because the model is not updated several times. In some cases DEFER is necessary because some groups of modifications do not have valid intermediate geometry.
-->(PD_NEW_C_LINE_COLOR)--|color|-->
PD_NEW_C_LINE_COLOR sets the color of construction lines created by the Parametrics module. This creation can occur when geometry is created with COPILOT turned on, when automatic constraint generation takes place, or when constraints are assigned.
-->(PD_NEW_C_LINE_LINETYPE)--|linetype|-->
PD_NEW_C_LINE_LINETYPE sets the linetype of construction lines created by the Parametrics module. This creation can occur when geometry is created with COPILOT turned on, when automatic constraint generation takes place, or when constraints are assigned.
-->(PD_NEW_C_LINE_VISIBILITY)--+--(VISIBLE)----+-->
| |
+--(INVISIBLE)--+
PD_NEW_C_LINE_VISIBILITY sets the visibility of construction lines created by the Parametrics module. This creation can occur when geometry is created with COPILOT turned on, when automatic constraint generation takes place, or when constraints are assigned.
-->(PD_NEW_POINT_COLOR)--|color|-->
This function specifies the color to be used for new points that are created by the system. This creation can occur in either the automatic constraint generator or when the user defines new PD_POINT and PD_POINT_ON constraints.
-->(PD_NEW_POINT_LINETYPE)--|linetype|-->
This function specifies the linetype to be used for new points that are created by the system. This creation can occur in either the automatic constraint generator or when the user defines new PD_POINT and PD_POINT_ON constraints.
-->(PD_NEW_POINT_VISIBILITY)--+--(VISIBLE)----+-->
| |
+--(INVISIBLE)--+
PD_NEW_POINT_VISIBILITY sets the visibility of points created by the Parametrics module. This creation can occur when geometry is created with COPILOT turned on, when automatic constraint generation takes place, or when constraints are assigned.
-->(PD_PARAM_ADD)--+---(ANGLE_PAR)----+---|parameter name|--->
| |
+---(LENGTH_PAR)---+
| |
+---(POINT_PAR)----+
| |
+---(USER_PAR)-----+
PD_PARAM_ADD adds a new parameter to the current part. The parameter must be one of four types: angle, length, point or user.
-->(PD_PARAM_FIX)--|parameter name|--+--------|number|----------+--->
| |
+--(')--|expression|--(')--+
| |
+----------('')------------+
PD_PARAM_FIX defines what the value of the named parameter will be during the next call to PD_RESOLVE.
Inputting a |value| causes the new value of that parameter to be the given value. The value must be either a number or a point, depending on the parameter type.
Inputting a quoted expression will cause the expression to be evaluated during subsequent calls to PD_RESOLVE. The expression can include references to other parameters. Any valid ME10 expression is allowed.
Inputting a null string, '', removes any previously defined value or expression for the parameter.
-->(PD_PARAM_INQ)----|parameter name|--->
PD_PARAM_INQ writes information about the parameter into the system inquiry array. It can then be retrieved with INQ (see INQ).
PD_PARAM_INQ set the following values:
+----------------------------------------------------------------------+ | function/command || result | +------------------+-------------+-------------------------------------+ | PD_PARAM_INQ | 1 | 130 (inq code) | | | 2 | 0 : Named parameter does not exist | | | | 1 : Named parameter does exist | | | 5 | Conversion factor from parameter | | | | units to system units | | | 6 | 0 : Length parameter | | | | 1 : Angle parameter | | | | 2 : User parameter | | | | 3 : Point parameter | |......................................................................| | if parameter type is not PD_POINT | |......................................................................| | | 3 | Current parameter value. | |......................................................................| | if parameter type is PD_POINT | |......................................................................| | | 3 | X coordinate of point parameter. | | | 4 | Y coordinate of point parameter. | +----------------------------------------------------------------------+
-->(PD_PARAM_REMOVE)----|parameter name|--->
PD_PARAM_REMOVE removes a parameter from the current part. The command will fail if the named parameter is used within an expression for another parameter or as the value for a constraint.
-->(PD_PARAM_SAVE)--->|output_spec|---->
PD_PARAM_SAVE saves the parameter settings to "output spec" ( see help for OUTPUT_SPEC for details). Output consists of a PD_PARAM_FIX command for each parameter. The file can be read with INPUT to restore the parameter settings.
-->(PD_PARAM_SHOW)---+--(ALL)---+-------------->
| |
+--(USER)--+
PD_PARAM_SHOW displays constraints which reference parameters. If USER is specified then only those constraints which reference parameters set by value will be displayed.
-->(PD_PREVIEW_COLOR)----|color|---->
PD_PREVIEW_COLOR is used to set the color of geometry displayed by subsequent calls to PD_RESOLVE PREVIEW.
-->(PD_RESOLVE)--+--(GENERATE)--+----------+-------------------+--->
| | | |
| +--(UNDO)--+ |
| |
+--(PREVIEW)----------------------------------+
| |
+--(REPLACE)---+----------+-------------------+
| | | |
| +--(UNDO)--+ |
| |
| +----(UNDO)------+ |
| V ^ |
+--(COPY)---|ref_pnt|---+---|move_pnt|---+----+
PD_RESOLVE is used both to automatically generate new constraints and to modify geometry based on the application of parameters and constraints.
The GENERATE option will generate new constraints until the geometry in the modify zone is completely constrained. UNDO can be used to remove these constraints. A side effect of generating new constraints is that new POINT elements might be created. The color and linetype of these points is defined with PD_NEW_POINT_COLOR and PD_NEW_POINT_LINETYPE.
The PREVIEW option will show the original geometry as it was before the command is invoked, while showing any geometry that would be modified by a call to PD_RESOLVE REPLACE in the color specified by PD_PREVIEW_COLOR. This option is a useful method of comparing original and modified geometry without actually modifying the geometry in the database.
The REPLACE option will replace all geometry in the modify zone as necessary to satisfy the parameters and constraints on the geometry. UNDO can be used to restore the geometry back to the state it had before the command was invoked.
The COPY option will first show the geometry after application of parameters and constraints and then allow the translation of the geometry to one or more new locations. The original geometry will be restored when the command is finished.
-->(PD_RESOLVE_MERGE_TOLERANCE)----|number|--->
This function specifies the absolute tolerance used during PD_RESOLVE to decide whether the modification should result in the merging of two or more points, or in the deletion of small elements. The merge process can be eliminated by setting this tolerance to a negative number. The initial setting is 0.000001 mm.
+----------------+------------+
v v ^
-->(PD_RIGID_ADD)--+--|rigid name|--+--|select|--+-->
This command is used to define rigid bodies, which is a collection of geometric entities which PD_SOLVE will translate and rotate as a group. No change of size or relative position will occur on members of a rigid body.
You can have as many rigid bodies as you desire. The rigid name can be any user string.
Members of a rigid body can be any geometric entity, including subparts and hatchings. Subparts will translate and rotate with the rigid body. Hatchings will rotate with the rigid body.
Rigid body membership is recorded as an info string on the member entity. The form of the info string is always "PD_RIGID " + |rigid name|.
-->(PD_RIGID_REFRESH_TABLE)--->
This command is used to synchronize the contents of the logical table, rigids.ltab, with the names of all rigid bodies in the current part. This synchronization is done automatically whenever PD_RIGID_ADD, PD_RIGID_REMOVE, or PD_RIGID_SHOW is invoked, or when the current part is changed. However, since a rigid body is simply an info string, which can be edited by other means, this command is occasionally useful in its own right.
+----------------+------------+
v v ^
-->(PD_RIGID_REMOVE)--+--|rigid name|--+--|select|--+-->
This command is used to remove members from rigid bodies.
+----------------+
v ^
-->(PD_RIGID_SHOW)--+--|rigid name|--+-->
This command is used to highlight the members of a rigid body.
-->(PD_SHOW)--+--------------+--+--(ALLTYPES)----------+----->
| | | |
+--(BANNED)----+ +--(PD_ANGLE_LINES)----+
| | | |
+--(NEW)-------+ +--(PD_COLLINEAR)------+
| | | |
+--(SYSTEM)----+ +--(PD_DIMENSION)------+
| | | |
+--(UNUSED)----+ +--(PD_DISTANCE)-------+
| | | |
+--(USED)------+ +--(PD_ELEM)-----------+
| | | |
+--(USER)------+ +--(PD_FILLET)---------+
| | | |
+--(VIOLATED)--+ +--(PD_HORIZONTAL)-----+
| |
+--(PD_MIRROR)---------+
| |
+--(PD_PARALLEL)-------+
| |
+--(PD_PERPENDICULAR)--+
| |
+--(PD_POINT)----------+
| |
+--(PD_POINT_ON)-------+
| |
+--(PD_SAME_DISTANCE)--+
| |
+--(PD_SAME_SIZE)------+
| |
+--(PD_SIZE)-----------+
| |
+--(PD_SLOPE)----------+
| |
+--(PD_SYM_LINE)-------+
| |
+--(PD_TANGENT)--------+
| |
+--(PD_VERTICAL)-------+
PD_SHOW is used to add a subset of the constraint icons to the display.
The set of constraints to be added can be restricted in two ways. First, an optional constraint kind modifier can be given. Second, a constraint type or ALLTYPES must be given.
The kind modifier is BANNED, NEW, SYSTEM, UNUSED, USED, USER, VIOLATED. BANNED constraints are those which the user has explicitly banned with the PD_FREE BAN command. NEW constraints are those constraints that are being added by a call to PD_RESOLVE GENERATE, which means that NEW is only useful while the PD_RESOLVE GENERATE command is displaying a message indicating the number of constraints added. SYSTEM constraints are those constraints added by previous calls to PD_RESOLVE GENERATE and unmodified by the user. UNUSED are those constraints that were not used by the last call to PD_RESOLVE to determine the new geometry but were satisfied. USED are those constraints that were used in the last call to PD_RESOLVE to determine the new geometry. USER are those constraints added by the user or system constraints that were modified by the user. VIOLATED are those constraints that were violated by the last call to PD_RESOLVE.
-->(PD_SHOW_CLEAR)--+--------------+--+--(ALLTYPES)----------+-----+--->
| | | |
+--(BANNED)----+ +--(PD_ANGLE_LINES)----+
| | | |
+--(NEW)-------+ +--(PD_COLLINEAR)------+
| | | |
+--(SYSTEM)----+ +--(PD_DIMENSION)------+
| | | |
+--(UNUSED)----+ +--(PD_DISTANCE)-------+
| | | |
+--(USED)------+ +--(PD_ELEM)-----------+
| | | |
+--(USER)------+ +--(PD_FILLET)---------+
| | | |
+--(VIOLATED)--+ +--(PD_HORIZONTAL)-----+
| |
+--(PD_MIRROR)---------+
| |
+--(PD_PARALLEL)-------+
| |
+--(PD_PERPENDICULAR)--+
| |
+--(PD_POINT)----------+
| |
+--(PD_POINT_ON)-------+
| |
+--(PD_SAME_DISTANCE)--+
| |
+--(PD_SAME_SIZE)------+
| |
+--(PD_SIZE)-----------+
| |
+--(PD_SLOPE)----------+
| |
+--(PD_SYM_LINE)-------+
| |
+--(PD_TANGENT)--------+
| |
+--(PD_VERTICAL)-------+
PD_SHOW_CLEAR is used to remove a subset of the constraint icons which are currently being displayed.
The set of constraints to be removed follows the same syntax is PD_SHOW.
Example:
PD_SHOW_CLEAR ALLTYPES
This is the simplest way to remove all constraint icons from the display.
-->(PD_SHOW_COLOR)----|color|---->
PD_SHOW_COLOR is used to set the color of constraint icons displayed by subsequent calls to PD_SHOW.
-->(PD_SHOW_LABEL_SIZE)---|size|--->
PD_SHOW_LABEL_SIZE is used to set the size of constraint icons displayed by subsequent calls to PD_SHOW.
+-----------<-------------+
| |
-->(PD_SHOW_MOVE_TEXT)--+--|id_pnt|---|move_pnt|--+-->
PD_SHOW_MOVE_TEXT is used to move the set of constraint icons from their current position to a new position. A set of constraint icons is all of the constraint icons attached to a particular geometry element. The new position will be used by all subsequent calls to PD_SHOW that cause constraint icons to be displayed for the element, as long as the current session is active.
-->(PD_SHOW_USE_POSTFIX)--+---(NO)--+--->
| |
+--(YES)--+
PD_SHOW_USE_POSTFIX is used to set the show mode for dimension constraints. If YES, the constraint value is displayed in the postfix field of the dimension. If NO, the constraint value is displayed in the main value field of the dimension.
+-------------------<-----------------------+
| |
-->(PD_USE_DIMENSION)--+--|parametric dimension|--|new dimension|--+---->
PD_USE_DIMENSION exchanges a parametric dimension with a non-parametric dimension. The parametric dimensions which are created when COPILOT is on may not be the preferred ones in all cases. A dimension may be created with the normal dimension commands and then swapped via PD_USE_DIMENSION so that it becomes a parametric dimension.
In order for an exchange to occur, both dimensions must control the same geometry.
+-----<------+
| |
-->(PD_ZONE_ADD)--+---------------+--+--|select|--+-->
| |
+--(NEIGHBORS)--+
PD_ZONE_ADD adds elements to the modify zone. If the NEIGHBORS qualifier is not given, then the elements added are the elements selected. If the NEIGHBORS qualifier is given then the elements added to the zone are the elements selected and any elements that share a model point with one of the elements selected.
The modify zone is the set of elements which might be modified by the PD_RESOLVE command.
+-----<------+
| |
-->(PD_ZONE_REMOVE)--+--|select|--+-->
PD_ZONE_REMOVE removes elements from the modify zone.
-->(PD_ZONE_SHOW)---->
PD_ZONE_SHOW highlights all elements in the current modify zone. The highlight is removed on the next screen redraw.
-->(PENSIZE)---|pensize|--->
PENSIZE specifies the current pensize for all new geometry except construction geometry and POINT symbols. By default, the current pensize is 0.
The pensize of geometry will keep its value and look the same when the geometry or the part or drawing to which the geometry belongs are scaled. The pensize attribute is therefore called "scale invariant".
Pensize and linesize (see LINESIZE function) are alternative values: geometry can either have a pensize or a linesize but it can never have both.
The PEN SIZE menu button displays a menu of commands for adding and deleting pensize types to the current dimension selection filter.
---->(PERMANENT_KNOBBOX)---->+------>(ON)----->+---->
| |
`------>(OFF)---->'
Default: OFF
If PERMANENT_KNOBBOX is turned on, the knobbox (if present) can be directly used for panning and zooming without interrupting the current command or function.
Returns an approximate value for pi (~3.14159265358979).
---->(PICK_VP_PNT)--->---|number|--->---|string|--->---|point|---->
Emulate interactive user pick in a specific viewport, defined by number and viewportname. To be used in conjunction with READ PNT function, which returns the viewportnumber (INQ 2) and name (INQ 301).
The PIXMAP_EDITOR function displays the PIXMAP BROWSER window. This window lists the pixmaps in the form of a table.
With the pixmaps editor displayed:
Commands in the pixmaps editor include:
-->(PIXMAP_LIST)--+-----(SCREEN)----------------------+---->
| |
'--+-----------+--|file specifier|--'
| |
+-(DEL_OLD)-+
| |
'-(APPEND)--'
PIXMAP_LIST lists the pixmaps information loaded in the current session.
SCREEN sends the output to the built-in editor (see EDITOR). Otherwise, the output is sent to the file specified. With DEL_OLD, a file of the same name is overwritten without any error message. With APPEND, the pixmaps list goes to the end of the named file, if it exists; otherwise, a new one is created. With neither DEL_OLD or APPEND option, if a file of the same name is present in the specified path, error is reported.
->(PLOT)->+------------->+->+----------------->+->+----------------->+--.
| | | | | | |
`->|offs_pnt|->' `->|rotate_angle|->' `->(AS_DISPLAYED)->' |
|
.----------------------------------------------------------------'
|
+--->(DEFAULT)--->|string|---.
| |
+<---------------------------'
|
`--->+----------->+--->+----------------->(ALL)---------------->+--+
| | | | |
`-->(OFF)--->' +------------->(CURRENT_WINDOW)--------->+ |
| | |
+---------------->|string|-------------->+ |
| | |
`--->(TWO_PTS)--->|ll pnt|--->|ur pnt|-->' |
|
,----------------------------------<-------------------------------'
|
+-------->-------+---+------->-------+---+--------->----------+-->
| | | | | |
+->-(COLOR_IMG)--+ +-->(BEST_IMG)--+ +-->(NORM_VIDEO)-----+
| | | | | |
'->-(BW_IMG)-----' '-->(LOW_IMG)---' '-->(REVERSE_VIDEO)--'
PLOT generates plot data which is usually sent to a spooler directly. The spooler program sends the plot data to the plotter device. The plot menu allows you to specify most of the plot options interactively. When you invoke a plot using the START PLOT entry in the plot menu, the PLOT command is called using the options set according to the highlighted items on the plot menus and according to the plot settings defined in the file "defaults".
rotate_angle: number (default 0) Gives the rotation angle of the drawing on the paper in current angular units. In the plot menu use ROTATE ANG to specify this angle.
DEFAULT Puts a string containing plot commands (HP-GL or HP-GL/2) into the plot data after initialization and before any drawing element is plotted. This is useful to change the plot speed or other global plotter parameters.
AS_DISPLAYED The drawing is to be plotted according to the show status of the current viewport, with construction geometry, spotlighting, vertex points, and part boxes. This option tells HOW to plot the drawing, but not WHAT to plot. In the plot menu use Curr Show in CONTENTS to set this option.
If AS_DISPLAYED is not specified, the model is plotted as a normal drawing suppressing vertex points, spotlighting, show changes, part boxes and construction geo, but including all geometry and dimensioning. In the plot menu use Drawing in CONTENTS to get a plot according to the standard drawing conventions.
OFF No paper advance before plotting.
ALL CURRENT_WINDOW string TWO_PTS ll_pnt, ur_pnt
This group of options tells WHAT to plot:
Resolution for HIGH Quality and DRAFT Quality are defined in plotdefs file. For HIGH Quality, the resolution value is 300 DPI. For DRAFT Quality, the resolution value is 150 DPI. This resolution value in plotdefs file can be modified for better quality. See Mustread_plotdefs.
->(PLOT)->+------------->+->+----------------->+->+----------------->+--.
| | | | | | |
`->|offs_pnt|->' `->|rotate_angle|->' `->(AS_DISPLAYED)->' |
|
.-------------------------------------------------------------'
|
|
`---->+----------------->(ALL)---------------->+---->
| |
+------------->(CURRENT_WINDOW)--------->+
| |
`--->(TWO_PTS)--->|ll pnt|--->|ur pnt|-->'
PLOT generates plot data which is sent to the Windows Print Manager for printing or plotting, or to the Windows Clipboard. The Print Manager spools the plot data to the physical device, and may offer you additional options at print time via its own window. Clipboard items can be pasted into other Windows applications. The plot menu allows you to specify most of the plot options interactively. When you invoke a plot using the START PLOT entry in the plot menu, the PLOT command is called using the options set according to the highlighted items on the plot menu and according to the plot settings defined in the file "defaults.mac".
rotate_angle: number (default 0) Gives the rotation angle of the drawing on the paper in current angular units. In the plot menu use ROTATE ANG to specify this angle.
AS_DISPLAYED The drawing is to be plotted according to the show status of the current viewport, with construction geometry, spotlighting, vertex points, and part boxes. This option tells HOW to plot the drawing, but not WHAT to plot. In the plot menu use Curr Show in CONTENTS to set this option.
If AS_DISPLAYED is not specified, the model is plotted as a normal drawing suppressing vertex points, spotlighting, show changes, part boxes and construction geo, but including all geometry and dimensioning. In the plot menu use Drawing in CONTENTS to get a plot according to the standard drawing conventions.
ALL CURRENT_WINDOW TWO_PTS ll_pnt, ur_pnt
This group of options tells WHAT to plot:
In this menu you can specify the plotters you want to use and the file handling. You can select from the list of predefined plot configurations. Each predefined configuration contains settings for the following :
Plotter Type Plot Destination Plot Default String Plot Macro To Execute
These settings are stored in the file "defaults".
The Plot Configuration menu can be turned on or off.
he plot menus allow the user to specify a set of plot parameters before starting the plot procedure. Screen dumps are also available from the plot menu. Use the plot configuration menu to select a predefined plot configuration first. The name of the selected plot configuration is indicated on the plot menu to the right of the START PLOT menu entry. If you want to invoke plots via the menu you should not try to set plot parameters by entering plot functions via the keyboard. The default values for the plot menus are defined in the file "defaults".
In this menu you can choose how the drawing will be plotted. There are options for :
Positioning the Drawing Setting the Plot Scale Setting the Plot Appearance Setting the Rotation Angle Selecting the Paper Size
The Plot Settings menu can be turned on or off.
--->(PLOTTER_TYPE)-->(ADD)--+
|
+-------------------------+
| +----------<----------<-------+
| | |
+---------->------------>+->+---------->---------->------->->|plotter names|->
| | | |
+---->----->+ | +->(FRONT_STRING)-->|string|->+
| | | | |
+->(HPGL)-->+->(CENTER)->+ +->(APPEND_STRING)->|string|->+
| | | |
+------->(HPGL2)-------->+ +->(NO_LINETYPE_ADJUST)------>+
| |
+------(HPGL2_RTL)-------+
| |
+------(POSTSCRIPT)------+
PLOTTER_TYPE specifies the type of plotter you want to use next. After selecting a new plotter you should reset the PLOT_TRANSFORMATION. If you are using the plot menu you have to specify the PLOTTER TYPE in the plot configuration menu. When you select a plot configuration the plotter type will be set accordingly and the PLOT_TRANSFORMATION will RESET to the plotters default.
For a list of compatible plotters, refer to your product Configuration Manual.
PLOTTER_TYPE ADD defines a new plotter with the specified plotter names. Plotter names have to be given as one string with one or more names for the plotter separated with a comma (,). The first name will be used for the plotter name inquire, all other names may be used as alternative names.
For the new plotter, you can specify the following options:
By default, a new plotter can use adjusted linetypes. Only if the new plotter does not support this feature or if the plotter has problems with this feature use (NO_LINETYPE_ADJUST) to disable the default. This option is necessary for the following plotters:
Thick lines (lines > 0) always use the adjusted linetypes feature even if NO_LINETYPE_ADJUST is specified.
Example:
PLOTTER_TYPE ADD
HPGL2 {Create an HPGL2 file}
NO_LINETYPE_ADJUST {Firmware bugfix for Laserjet III}
FRONT_STRING (chr(27)+"E"+ {Reset Printer}
chr(27)+"&l3o0E"+ {Set to Landscape mode}
chr(27)+"*p45Y"+ {Set cursor to max lower left corner}
chr(27)+"*ct5710Y"+ {Set cursor pos and length to 8176 dcipnt}
chr(27)+"%0B") {Enter to HPGL/2 mode}
APPEND_STRING (";"+ {Terminate HPGL files for HPGL2 devices}
chr(27)+"E") {Reset Printer}
'LASERJET/III/A4,LJ/III/A4' {Name of the new added printer}
-->(PLOT_AUTO_ROTATE)----+--(ON)---+----> | | +--(OFF)--+
If PLOT_AUTO_ROTATE is set to OFF the string "5,1;" will be added to each HP-GL/2 plot file immediately after plot initialization (ESC%-1B BP). This option allows you to disable the auto - rotate feature that is part of the firmware on some raster plotters. By default, the auto - rotate feature is active if no specific initialization is sent ( ESC%-1B BP5,1; ).
The auto - rotate feature tries to minimize the paper use by rotating the plot. This feature might be very nasty with small drawing sizes like DIN A4 on a bigger paper size like DIN A0 because it does not allow to place drawings side by side on the paper.
Examples:
Auto - Rotate active: (default setting for HP-GL/2 or PLOT_AUTO_ROTATE is set to ON)
-----------------------------------
| ___________ ___________ |
| | | | | | DIN A0 Page
| | DIN | | DIN | |
| | A4 | | A4 | |
| |___________| |___________| |
| |
-----------------------------------
Auto Rotate disabled: (PLOT_AUTO_ROTATE is set to OFF)
If all three DIN A4 plots are generated with PLOT_AUTO_ROTATE OFF they will fit in one form feed of the plotter.
-----------------------------------
| _______ _______ _______ |
| | | | | | ||
| | | | | | || DIN A0 Page
| | DIN | | DIN | | DIN ||
| | A4 | | A4 | | A4 ||
| | | | | | ||
| |_______| |_______| |_______||
| |
-----------------------------------
Currently only the HP DesignJet Serie and the HP Electrostatic plotters support the auto - rotate feature. For more information on this feature please refer to the manual delivered with your plotter.
--->(PLOT_CENTER)--->+--->(ON)---->+--->
| |
`--->(OFF)--->'
PLOT_CENTER centers the drawing in the plotter viewport: Center (ON) or not center (OFF). See PLOT_VIEWPORT. If you are using the plot menu you have to specify the POSITION there accordingly.
--->(PLOT_DESTINATION)--->+---------------->+--->|plot destination name|--->
| |
`--->(DEL_OLD)--->'
PLOT_DESTINATION defines where the plot should be sent. You enter the name of a plot file. You must enter DEL_OLD to delete an existing plot file.
A legal plot destination name may start with the UNIX pipe symbol '|' to send the plot data directly to a UNIX process. This provides a simple way to transfer the plot data to a spooler other than the ME plotspooler.
Example: '| np -q ColorElectro' will send the plot data directly to the HP OpenSpool spooler with a configured queue ColorElectro. (See HP OpenSpool). You will get a error message when the transfer to the specified UNIX process was not successful (for example when using wrong options for the UNIX process). The DEL_OLD option has no effect when piping a plot.
If you are using the plot menu you have to specify the PLOT DESTINATION in the plot configuration menu. There you also can specify the DEL_OLD option via the Delete Old menu entry. When you select a plot configuration the PLOT DESTINATION, the Delete Old and Generate Name option will be set according to the selected configuration.
--->(PLOT_FORMAT)--->|fwidth|--->|fheight|--->
PLOT_FORMAT defines the maximum plotting area (hard limits) which can be used. See PLOT_VIEWPORT for further information. The width and height is specified in user units.
If you are using the plot menu you have to specify the plot format using the PAPER SIZE entry in the plot menu. For all predefined paper sizes (A-E, A4-A0) the valid sizes are read from the file "plotdefs". See plotdefs for a detailed description of the file format.
--->(PLOT_IMAGE_QUALITY)--->|Color palette|--->|Monochrome Resolution|--,
|
,----------------------------<---------------------------'
|
`--->|Color Resolution|--->|Scaling|--->|Compression|------>
PLOT_IMAGE_QUALITY defines the Color palette, Monochrome Resolution, Color Resolution, Scaling and Compression supported by the device.
See PLOTDEFS for further information.
--->(PLOT_LINETYPE_LENGTH)--->+--->(MIN_DIST_FACTOR)---.
v |
+<-----------------------'
|
+--->|length1|---> ... --->|length7|--->+------->
| |
+----->|linetype|---------->|length|--->'
PLOT_LINETYPE_LENGTH specifies the length of the pattern (user units) for each linetype. You can enter seven different lengths, one for each linetype except solid; see LINETYPE for the correct order. You can also enter a single linetype/length pair, or, with ALL, a single length for all linetypes.
The qualifier MIN_DIST_FACTOR is for plotting of elements with a pensize or linesize only. With MIN_DIST_FACTOR, you can set a minimal distance between the subpatterns of a linetype for each linetype. This distance is measured as a percentage of the pensize or linesize of the current element. The default value for all linetypes is 0.25.
If you are using the plot menu you have to specify the plot linetype length using the LTYPE LEN entry in the plot menu.
-->(PLOT_PEN_TABLE)--->|transformation row for solid|--->.
.<-------------------------------------'
`--->|transformation row for dashed|--->.
.<-------------------------------------'
`--->|transformation row for long_dashed|--->.
.<-------------------------------------------'
`--->|transformation row for dot_center|--->.
.<------------------------------------------'
`--->|transformation row for dash_center|--->.
.<-------------------------------------------'
`--->|transformation row for phantom|--->.
.<---------------------------------------'
`--->|transformation row for center_dash_dash|--->.
.<------------------------------------------------'
`--->|transformation row for dotted|------------->
PLOT_PEN_TABLE controls the mapping of linetypes and colors to plotter pens and plotter linetypes. For each linetype, in the above order, you enter a string describing the transformation.
The transformation row for a linetype is a string consisting of 8 pairs of characters, one for each color. The first character in the pair names the plotter linetype, ('A'...'H' for solid to dotted) and the second gives the pen number. The character pairs can be delimited by blanks.
PLOT_PEN_TABLE
{BLACK RED GREEN YELLOW BLUE MAGENTA CYAN WHITE}
{ 0 1 2 3 4 5 6 7}
{A SOLID} 'A0 A2 A4 A3 A7 A6 A5 A1'
{B DASHED} 'B0 B2 B4 B3 B7 B6 B5 B1'
{C LONG_DASHED} 'C0 C2 C4 C3 C7 C6 C5 C1'
{D DOT_CENTER} 'D0 D2 D4 D3 D7 D6 D5 D1'
{E DASH_CENTER} 'E0 E2 E4 E3 E7 E6 E5 E1'
{F PHANTOM} 'F0 F2 F4 F3 F7 F6 F0 F1'
{G CENTER_DASH_}'G0 G2 G4 G3 G7 G6 G5 G1'
{H DOTTED} 'H0 H2 H4 H3 H7 H6 H5 H1'
Use PLOT_TRANSFORMATION for new macros.
--->(PLOT_SCALE)--->+--->|scale factor|--->+--->
| |
`------>(AUTO)-------->'
scale factor: number
PLOT_SCALE sets the factor by which the entire drawing (including text, dimensioning, and symbols) is scaled before being plotted.
If you are using the plot menu you have to specify the plot scale using the SCALE entry in the plot menu. You can also specify the AUTO option via the Fit menu entry.
---->(PLOT_STOP_ON_ERROR)---->+------>(ON)----->+---->
| |
`------>(OFF)---->'
This function controls the plot behavior when a drawing does not fit in the plot area. The default value is OFF, which means that the drawing is plotted even if the plot does not fit. If set to ON and this error occurs, plotting is canceled.
--->(PLOT_TRANSFORMATION)--->+---------------->(RESET)---------------->+-->
.<--------------------------' ^
+------------------>(ALL)---------------------. |
| v |
`-->|first linetype|--+-->|second linetype|---+ |
v | |
.<--------------------+<----------------------' |
| |
+------------------>(ALL)------------------------. |
| | |
+----------------->|color|---------------------->+ |
| | |
`--->|first red int|---->|second red int|---. | |
.<------------------------------------------' | |
`-->|first green int|-->|second green int|--. | |
.<------------------------------------------' v |
`-->|first blue int|---->|second blue int|------>+ |
.<-----------------------------------------------' |
| |
+------------------>(ALL)------------------------. |
| | |
+--->|first pensize|---->|second pensize|------->+ |
| | |
+<-----------------------------------------------' |
| |
| |
+------->(SAME)------>+-+-------------------------------+-->|pen|-----'
| ^ | ^
`--->|new linetype|---' `--->(PENWIDTH)--->|penwidth|---'
The PLOT_TRANSFORMATION function can be used more than once to specify different transformations. If the last specified plot transformation includes the range of a previously defined plot transformation, the previous transformation is overwritten by the new one. All elements which results in a plot transformation with pen equal 0 are not plotted. The specified pen number must be valid with respect to the plotter to be used.
The default plot transformation (accomplished by PLOT_TRANSFORMATION RESET) depends on the plotter language (HPGL or HPGL2) which is set for the current plotter:
HP-GL (HP-GL/2)
PLOT_TRANSFORMATION ALL ALL SAME 1 (1)
PLOT_TRANSFORMATION ALL BLACK SAME 0 (0)
PLOT_TRANSFORMATION ALL RED SAME 2 (2)
PLOT_TRANSFORMATION ALL GREEN SAME 4 (3)
PLOT_TRANSFORMATION ALL YELLOW SAME 3 (4)
PLOT_TRANSFORMATION ALL BLUE SAME 7 (5)
PLOT_TRANSFORMATION ALL MAGENTA SAME 6 (6)
PLOT_TRANSFORMATION ALL CYAN SAME 5 (7)
PLOT_TRANSFORMATION PHANTOM CYAN SAME 0 (0)
Due to a limitation of some plotter devices PHANTOM and CENTER_DASH_DASH line types are plotted the same by default.
PLOT_TRANSFORMATION settings are overwritten if another plotting device is chosen.
The PLOT_TRANSFORMATION function can be used to assign a display color to a plot pen and penwidth. For example, the following results in all red lines being plotted with a penwidth of 5mm.
PLOT_TRANSFORMATION ALL RED ALL SAME PENWIDTH 5 1
| | | | | | |
1 2 3 4 `----' 6
5
1 - All linetypes
2 - Only red objects
3 - All screen pensizes
4 - Linetype should stay the same
5 - Assign a penwidth of 5mm
6 - Use pen number 1
The PLOT_TRANSFORMATION function is the recommended way to assign pensizes to pens. An alternative method is to assign penwidths directly as in the plot default parameter:
Set_sys_plot_default ( 'NP8;WU;PW0.3750,1;PW0.6875,2;PW0.1875,3;PW0.2500,4;'
+ 'PW0.3125,5;PW0.5000,6;PW1.0000,7;')
However, this applies only if the drawing does not contain geometry with a pensize and if you do not use PLOT_TRANSFORMATION to produce the pensize.
--->(PLOT_TRANSFORMATION)--->+---------------------------------------->+-->
.<--------------------------' ^
+------------------>(ALL)---------------------. |
| v |
`-->|first linetype|--+-->|second linetype|---+ |
v | |
.<--------------------+<----------------------' |
| |
+------------------>(ALL)------------------------. |
| | |
+----------------->|color|---------------------->+ |
| | |
`--->|first red int|---->|second red int|---. | |
.<------------------------------------------' | |
`-->|first green int|-->|second green int|--. | |
.<------------------------------------------' v |
`-->|first blue int|---->|second blue int|------>+ |
.<-----------------------------------------------' |
| |
+------------------>(ALL)------------------------. |
| | |
+--->|first pensize|---->|second pensize|------->+ |
| | |
+<-----------------------------------------------' |
| |
| |
+------->(SAME)------>+-+-------------------------------+-->|pen|-----'
| ^ | ^
`--->|new linetype|---' `--->(PENWIDTH)--->|penwidth|---'
The PLOT_TRANSFORMATION function can be used more than once to specify different transformations. If the last specified plot transformation includes the range of a previously defined plot transformation, the previous transformation is overwritten by the new one. All elements which results in a plot transformation with pen equal 0 are not plotted. The specified pen number must be valid with respect to the plotter to be used.
The default plot transformation (accomplished by Plot_default_transformation) is:
PLOT_TRANSFORMATION ALL ALL SAME 1 PLOT_TRANSFORMATION ALL BLACK SAME 0 PLOT_TRANSFORMATION ALL RED SAME 2 PLOT_TRANSFORMATION ALL GREEN SAME 3 PLOT_TRANSFORMATION ALL YELLOW SAME 4 PLOT_TRANSFORMATION ALL BLUE SAME 5 PLOT_TRANSFORMATION ALL MAGENTA SAME 6 PLOT_TRANSFORMATION ALL CYAN SAME 7 PLOT_TRANSFORMATION PHANTOM CYAN SAME 0
Due to a limitation of some plotter devices PHANTOM and CENTER_DASH_DASH line types are plotted the same by default.
PLOT_TRANSFORMATION settings are overwritten if another plotting device is chosen.
Three general-purpose plot transformations are defined on the PLOT OPTION block of the PLOT menu. These are:
Plot_black_and_white -- Suitable for output to a black and white device.
All line colors are mapped to black, but given
different widths based on color.
Plot_pen_color -- Suitable for output to pen plotters. All colors
are mapped to one of eight pen colors. White elements
are mapped to black.
Plot_true_color -- Suitable for output to color printers. No
transformation is done and TRUE_COLOR_PLOTTING is
enabled.
The PLOT_TRANSFORMATION function can be used to assign a display color to a plot pen and penwidth. For example, the following results in all red lines being plotted with a penwidth of 5mm.
PLOT_TRANSFORMATION ALL RED ALL SAME PENWIDTH 5 1
| | | | | | |
1 2 3 4 `----' 6
5
1 - All linetypes
2 - Only red objects
3 - All screen pensizes
4 - Linetype should stay the same
5 - Assign a penwidth of 5mm
6 - Use pen number 1
--->(PLOT_VIEWPORT)--->+-------------------->(FORMAT)----------------->+-->
| |
`-->|xoffset|->|yoffset|->|vwidth|->|vheight|-->'
PLOT_VIEWPORT locates the plotter viewport (soft limits) within the maximum plotting area (hard limits, specified by PLOT_FORMAT). The soft limits must as a minimum partially overlap the hard limits. The layout is as follows:
physical paper area
+___________________________________________________________________
| maximum plotting area (hard limits) |
| +_____________________________________________________________ |
| | ^ | |
| | | | |
| | plotter viewport (soft limits) | | |
| | +__________________ P2 | | |
| | |<----vwidth----->| ^ | | |
| | | | | | | |
| | ^y | vheight | | |
| | | x | | | | |
| |<------xoffset--------->|___>_____________| v fheight| |
| | P1 ^ | | |
| ^y | | | |
| | yoffset | | |
| |(0,0) x | | | |
| |______>_________________v_______________________________v___| |
| <------------------------fwidth------------------------------> |
|__________________________________________________________________|
FORMAT means that the soft limits should be the same as the hard limits. If you are using the plot menu the FORMAT option is used.
Returns a 2D point (vector) with a length defined by the first and an angle to the X axis defined by the second argument.
Returns a 2D point (vector) with a x-coordinate defined by the first and a y-coordinate defined by the second argument.
Returns a 2D point with an X-coordinate defined by the first, a Y-coordinate defined by the second, and a screen defined by the third argument.
Returns a 3D point (vector) with an x-coordinate defined by the first, a y-coordinate defined by the second, and a z-coordinate defined by the third argument.
-->(POINT)--+-->|point|--+-->-----------------------------------------+--->
| ^ | |
| '------------' ,----<---, |
| | | |
+-(MIX)->--|pnt1|->--|pnt2|->-+-|frac|-+---->---------------+
| |pnt | |
| |
`->(ASSIST)-------------------------------------------------'
POINT creates point elements. You indicate where the element should go either directly or with MIX. MIX takes two (ordinary) points and generates a point element, either with a fraction or a third point. With a fraction, MIX generates the point pnt1 + frac * (pnt2 - pnt1). With a third point, MIX uses the perpendicular projection of this point on the imaginary infinite line between the first two points.
The ASSIST qualifier switches on user assistance (COPILOT command). Additional graphical feedback and creation methods are then available. See the COPILOT command for more information.
---->|number|---->( , )---->|number|---->
point_3d token
---->|number|---->( , )---->|number|---->( , )---->|number|---->
A point is given by X,Y coordinates, a point_3d is given by X,Y,Z coordinates.
---->(POLYELEM)--|startpoint|--+--|elem|--+-->(END)
| |
`----------'
This command lets you create a polyline from existing elements. You can then treat the polyline as a single element and modify it accordingly. The POLYELEM command applies to lines, arcs, fillets, and chamfers. However, it does not apply to elements having different line attributes.
The POLYELEM command works in the same way as the EQUIDISTANCE command.
--->(POP_DOWN_LTAB)--|name|-->
Causes the named logical table to "pop down". Pop down actions are unbuffered as opposed to pop up actions.
--->(POP_UP_LTAB)--|name|-->
Causes the named logical table to "pop up" at the next available opportunity. Pop up requests are buffered until the users is prompted for interactive input.
Returns the first position of a substring (second argument) within a string (first argument). If the substring is not contained in the string, returns 0.
---->(PRE_VIEW)----+----| ON |------+----------->
| |
`----| OFF |-----'
| |
`---|filename|---'
This command lets you enable/disable preview and preview a file. When store command is issued and if preview is enabled, preview data will also be stored in the file. If preview is disabled during store, preview data will not be stored.
You can preview the contents of an MI file by specifying the file name. The preview image will be displayed in a viewport placed to the left of the History table of File Browser.
--(PRINT_TABLE)-+->|table_id|-+-> | | +-->(ALL)---->+
This function allows you to print a display table in a file.
A Few Simple Problems and their Solutions:
Cannot draw any geometry (or construction geometry).
Hatching not visible.
Cannot turn on the grid.
Cannot select an element (computer beeps).
The Process Control menu has two submenus :
Logfile List to Review menu Logfile List to Delete menu
---->(PROMPT_LIST)---->+------>(ON)----------->+---->
| |
+------>(OFF)---------->+
| |
+------>(CLEAR)-------->+
| |
+---->|output_spec|---->+
The PROMPT_LIST facility may save up to 500 system prompts in internal memory. If more prompts are generated, the oldest are overwritten.
Options:
ON Enables saving of prompts (default).
OFF Disables saving of prompts.
CLEAR Clears the internal prompt list memory.
output_spec Outputs the internal prompt list memory to the specified
destination.
The PRT_EDITOR function displays the PART STRUCTURE EDITOR window. This window lists the parts and subparts.
With the parts editor displayed:
Commands in the parts editor include:
Shared parts within shared parts are shown as ##1.
The parts tree can be collapsed and expanded by picking the iconify/deiconify column. This is useful if you have a large assembly and do not want display nested parts.
,--------------,
| |
v |
-->(PUNCH_HOLE)-->-+--->|point|---+-->
PUNCH_HOLE makes holes in an existing hatch for the identified dimension texts or ordinary texts. Later changes to the dimension text or ordinary text (such as STRETCH) do not affect the size or position of the hatch hole.
-->(PURGE_FILE)->|filename|->+-+------------------>+->+->+-->(CONFIRM)->+->
| ^ | ^ | ^
| | | | | |
| | v | v |
| +<-|expr|-(SELECT)<-+ | '-->(SCREEN)-->'
| |
v |
'--->(RECURSIVE)-------->'
|expr|
--->|item|-------+-------->+------>|value|------>
| |
+->(=)--->+
| |
+->(<>)-->+
| |
+->(>)--->+
| |
+->(<)--->+
| |
+->(>=)-->+
| |
+->(<=)-->+
PURGE_FILE purges the specified files from the mass storage medium. The file 'hp_catfile' ('hp_cat.fil' in case of MS Windows) is considered to be a system file and cannot be purged with this function.
Wildcards can be used in filenames. See SELECT (the entry in this help file) for a description of wildcards.
See CATALOG (the entry in this help file) for a description of the SELECT option. See DEFINE_CATALOG for a description of |expr|.
With the RECURSIVE option you can purge files, empty directories and entire non empty directories (that means trees). Without the RECURSIVE option you can purge only files and empty directories.
The option SCREEN enters the built-in editor (see EDITOR) and allows you to verify the list of selected files and directories; any changes in the screen are ignored. With an unsuccessful exit (STOP/BREAK in Unix and ESC in MS Windows) from the editor you do not purge anything.
+<-----------------+
| |
---->(PUT_PROPERTIES)---->+---->|select|---->+---->
PUT_PROPERTIES changes the properties (color, linetype, etc) of the selected elements to be the current ones. For a complete list of which properties are affected, see GET_PROPERTIES.