What is the maximum number of characters allowed in a
Pro/ENGINEER object name?
How can upper case characters be used in Pro/ENGINEER
object names?
Is a default config.pro file created when Pro/ENGINEER
is installed?
Where does Pro/ENGINEER look for config.pro files?
After config.pro is edited, why aren't the changes reflected?
After config.pro is edited, is it necessary to restart
Pro/ENGINEER?
What is the difference between config.pro and config.sup?
Is there a limitation on the number of characters that
can be included in a config.pro entry?
Where are Pro/ENGINEER objects stored when File, Save...
is selected?
What does File, Save As... do?
What does File, Backup... do?
What does File, Rename... do?
What does File, Erase, Current... do?
What does File,
Erase, Not Displayed... do?
What does File,
Instance Operations do?
Does Pro/ENGINEER overwrite existing objects when saving
to disk?
What does the object version number indicate?
Does Pro/ENGINEER offer an auto-save function?
What happens if I run out of disk space while saving my
objects?
What is the difference between File, Erase and
File,
Delete?
Why is the following message given: "Check disk space
and write access?"
Why is the following message given: "PDM database object
must be renamed by Pro/PDM application"?
Why aren't part files saved when File, Save is
selected in Sketcher?
Does Pro/ENGINEER save all components each time an assembly
is saved?
Where does Pro/ENGINEER save part files that are assembled
from a directory different than the current working directory?
What happens during storage of an assembly if is dependent
part files are located in a write protected directory?
Why can't an assembly be retrieved after clearing it from
memory or after starting a new session of Pro/ENGINEER?
How does File, Save As function in Assembly mode?
Why do parts intersected by assembly features require
renaming before they can be saved?
What does the config.pro option "override_store_back"
do?
What does the config.pro option "save_object_in_current"
do?
What is the preferred method to make a copy of an assembly?
How can the orientation of the default view be changed?
How must Pro/ENGINEER be configured to recognize a Spaceball?
How can the quality of a shaded model be increased?
When a shaded model is spun, why does it revert back to
wireframe?
How can a postscript file of a shaded model be created?
Why aren't surface features displayed when the model is
shaded?
How is a color map file stored to disk?
Where does the color.map file need to be located in order
for Pro/ENGINEER to recognize it?
How many different colors can be defined and stored to
the color.map file?
Why is the Transparency menu selection not available?
When a color is assigned to a part in Assembly mode, why
is the color not reflected in Part mode?
What is the File, Working Directory.. menu selection
used for?
What is the Window, Open System menu selection
used for?
Why do the Pro/ENGINEER windows become inaccessible after
Window,
Open System is selected?
In which directory does Pro/ENGINEER create trail files?
Why is Pro/ENGINEER unable to execute a trail file with
the filename "trail.txt"?
What would cause a trail file to go out of sequence?
How can a trail file stop after each menu pick?
How can a trail file pause momentarily after each menu
pick?
How can the size of the Pro/ENGINEER working window be
controlled?
How can the fonts in the Pro/ENGINEER menus be changed?
How can the default location of the Pro/ENGINEER working
window be changed?
What would cause a mapkey to not work properly when it
is executed?
Where is the mapkey functionality documented?
Is there a limitation in the number of characters that
can be included in a mapkey?
How can a mapkey be defined to turn datum planes on and
off?
Why are mapkeys not recognized in the config.sup file?
Can keyboard function keys be used in a mapkey?
How can a mapkey call another mapkey?
Where is there detailed documentation on the menu_def.pro
file?
Where does Pro/ENGINEER look for menu_def.pro files?
How can a menu pick be removed from a menu?
Why doesn't a menu_def.pro menu selection work when it
is picked?
How can a new menu selection be placed at the top of a
menu?
How can the names of family table items (features, dimensions)
be changed so that the names that appear in the column headings are more
descriptive?
Is there a limit to the number of rows and/or columns
that can be included in a family table?
How can negative dimension values be entered in a family
table?
What does it mean to have nested instances?
What are .ptd and .idx files? Can they be deleted?
What should be done if a regeneration failure is encountered
during Verify?
How can the listing of all instances be prevented from
appearing in the menus when retrieving an object using File, Open?
How can a part or assembly instance be added to a Pro/ENGINEER
drawing as a drawing model?
What happens to the generic and all other instances if
features are created on a part or assembly instance?
In an assembly family table, how can components be replaced
with other part instances from the same family table?
How can part features and dimensions be controlled by
an assembly family table?
What is meant by a parent-child relationship?
Can a feature have more than one parent?
Can a feature have more than one child?
What will happen to a child if a parent is deleted or
suppressed?
How can a list of all parents and/or children of a specific
feature be obtained?
Can Pro/TABLE be utilized without running Pro/ENGINEER?
How can the width of the Pro/TABLE columns be modified?
After using Pro/TABLE, why does system speed decrease?
Is there a limit on the number of rows and columns that
can be used in the Pro/TABLE editor?
Pro/MECHANICA motion analysis run fails
The Pro/MECHANICA integrated mode does not work (FEM mode only available)
Thirty one (31) characters can be used in Pro/ENGINEER object names. This number does not include the extension, i.e., .prt, .asm, .drw, or the object version number, i.e., .1, .2, .3.
Upper case characters cannot be specified in Pro/ENGINEER object file names. Upper case characters can be specified during object creation, however, the file will be written to disk using lower case characters only.
When Pro/ENGINEER is initially installed, there is no default config.pro file that is created automatically. However, a large number of the options do have default values which are used unless the option setting is changed in a config.pro file. The Configuration Options section of Pro/HELP lists the default config.pro option values in italics. There are two methods that can be used to create a config.pro file. The first method is to utilize any text editor, vi for example, and manually create the file. Each option should have its own line in the file, with the format being {Option Value}. The second method is to use the Preferences dialog box within Pro/ENGINEER, which can be accessed by selecting Utilities, Preferences... When you exit the dialog box, the config.pro file will be written to your local directory. See the Suggested Technique for Using the Preferences Dialog Box for a detailed description of the functionality for this new dialog.
Pro/ENGINEER looks for config.pro files in 3 different directories in the following order:
After config.pro is edited, the Add/Change and Apply buttons must be selected in the Preferences dialog box in order for the modifications to be reflected in the Pro/ENGINEER session, or Pro/ENGINEER can be restarted. Be aware that some config.pro options require Pro/ENGINEER to be restarted in order for config.pro modifications to be reflected.
After config.pro is edited, the Apply button must be selected
in the Preferences dialog in order for the modifications to be reflected
in the Pro/ENGINEER session, or Pro/ENGINEER can be restarted. Modifications
to the following config.pro options require Pro/ENGINEER to be restarted:
There are two main differences between config.pro and config.sup.
Unlike config.pro, config.sup can only be located in the loadpoint/text directory.
Config.sup options cannot be overridden by options found in any other config.pro. Also, items contained in the config.sup can only have one entry per option. Keeping this in mind, it is important that items which can have multiple entries, such as "mapkey", "search_path", and "def_layer" are not specified in config.sup.
Each line in config.pro is limited to 80 characters. Environment variables can be used to specify config.pro "search_path" values containing more than 80 characters. Refer to Configuration Options in Pro/HELP for details.
*Where are Pro/ENGINEER objects stored when File, Save is selected?
By default, Pro/ENGINEER objects will be stored to the current working directory.
If the working directory is changed using File, Working Directory, Pro/ENGINEER objects will be saved to the new directory.
If a Pro/ENGINEER object is retrieved from a directory other than the current working directory, Pro/ENGINEER will save the object back to the directory from which it was retrieved. If the user does not have write permission in that directory, the object will not be saved unless the config.pro option "save_object_in_current" is set to "yes".
File - Save As will make a copy of a specified Pro/ENGINEER object using a new name. List the object that is to be copied in the Model Name space in the Save As dialog box, the current object being the default. In the New Name space, a new file name should be specified. Pro/ENGINEER will create this object in the current working directory.
File, Backup can be used to save Pro/ENGINEER objects to a specified directory. The object will be saved in the specified directory using the original filename(s).
File, Backup in Assembly, Drawing, or Manufacturing modes will save all related objects to the specified directory.
File, Rename is used to change the name of Pro/ENGINEER objects in memory and on disk. Pro/ENGINEER will rename all versions of the object being renamed.
When renaming an object that was retrieved from directory other than the current working directory, the renamed object will be saved in the directory from which the object was retrieved.
File, Erase is used to clear the specified object from workstation memory. This functionality will not remove objects from disk. Objects referenced by an active assembly or drawing can not be erased.
A list of objects in the current model will then be displayed.
Only the current top level model (i.e.. assembly or drawing) can be erased,
and selected objects as well.
File, Erase, Not Displayed is used to erase all objects from the current session, except for those that are currently displayed and any objects referenced by the displayed objects.
For example, if an assembly instance is being displayed at the time Erase, Not Displayed is selected, the instance, the instance's generic, and it's components will not be erased.
There is a config.pro option related to File, Erase, Not Displayed called "prompt_on_erasenotdisp".
yes (default) - a message window for each eligible object in question appears, asking if you want to first save the object before it is erased.
no - the system will immediately erase all eligible objects.
File, Instance Operations will save a particular instance of a part or assembly in a separate file called an " instance accelerator file" (suffix ".xpr" for a part, ".xas" for an assembly). This file is used to retrieve particular instances quickly from disk rather than having to first retrieve the generic into memory, selecting the particular instance according to the family table, and then regenerating. Therefore, with this functionality the amount of time that it takes to retrieve an instance of a part or assembly from disk can be considerably reduced. The trade off is that more disk space will be used to store the accelerator files.
When File, Instance Operations is selected, the INST DBMS
menu appears with the following options :
InstIndex: create or update the Instance Index file for a specified directory
Update Accel: create or update accelerator files for all instances currently in session
Purge Accel: examine each instance accelerator file and delete it if it is not current with the generic
SaveAccelEnv: brings up the SV INST ACC menu
When SaveAccelEnv is selected the SV INST ACC menu appears with
the following options:
none (default): the system does not save the instance in a file separate from the model.
always: the system always saves the instance in a separate file
explicit: the system saves the instance in a separate file only when the instance is explicitly saved.
The config.pro option "save_instance_accelerator" can also be used to control
instance accelerator files. The values for this config.pro option are also
none (default), always, explicit. When you bring up the SV INST ACC menu,
one of the options will be highlighted to reflect the last setting. That
setting could have been either loaded from a configuration file or selected
previously from this menu.
Pro/ENGINEER will not overwrite existing objects while saving to disk. Objects are saved to disk with an object version number after the file extension. Pro/ENGINEER will create a new object file each time the object is saved, monotonically increasing the version number each time.
Example: A part called valve.prt will be initially written to disk as valve.prt.1. Subsequent storage of this object will result in the files valve.prt.2. valve.prt.3, etc. When an object is retrieved and the directory contains multiple versions of the same object, the object with the highest version number will be retrieved.
The object version number indicates the number of times the object has been stored. Objects are saved to disk with an object version number after the file extension. Pro/ENGINEER will create a new object file each time the object is saved, monotonically increasing the version number each time.
Example: A part called valve.prt will be initially written to disk as valve.prt.1. Subsequent storage of this object will result in the files valve.prt.2. valve.prt.3, etc. If the directory is purged, the object with the highest version will remain.
When a top-level object is retrieved (for example, an assembly drawing), it always retrieves the most recent version of the assembly and its parts. Therefore, the version of the drawing does not necessarily have to have the same version number as the part or assembly. This will frequently be the case when several different users are working on the same files.
This wouldn't cause a problem unless a user deletes or redefines a feature that is used as a reference by some other object. For example, if a feature is deleted from a part that is used for assembling another component in an assembly, then that component will fail placement when the assembly is retrieved, and must be redefined. Another example is when planar surfaces are used to orient the model in a drawing view, and the feature is then deleted or suppressed. This will result in the message, "model geometry for drawing view is missing", and the view will revert to an isometric orientation, and must be re-oriented (using the default datum planes to orient the views whenever possible will help to prevent this).
The best method for avoiding these situations is to use a database management product that will manage revision changes made to parts/assemblies/drawings. Without a system like this, any user can change any model, regardless of what other users are doing.
Auto-save functionality is not currently implemented in Pro/ENGINEER. The "prompt_on_exit" config.pro option can be utilized to prompt the user to save objects in session before exiting Pro/ENGINEER.
If available disk space is depleted during storage, Pro/ENGINEER
will issue the message:
"object_name could not be saved: Check disk space or write access. Error in storage.
Check previous message (then press Enter):"
Pro/ENGINEER will not save any portion of the object to disk. Disk
space must be made available before the object can be saved.
File, Erase removes the object from workstation memory. The object is not removed from disk.
File, Delete removes either old versions or all versions of the object and all associated objects from disk. It is recommended to approach this menu selection with a great deal of caution. Creating backup copies of Pro/ENGINEER objects is considered good practice and can reduce the effect of accidental removal of data.
The message "Check disk space and write access" is given if the amount of disk space required to save the object exceeds available disk space or if the user does not have write access to the specified directory.
By default, Pro/ENGINEER will not allow Pro/PDM objects to be renamed within Pro/ENGINEER. The config.pro option "let_proe_rename_pdm_objects" set to "yes" will allow Pro/ENGINEER to rename Pro/PDM objects.
Warning: Objects renamed in Pro/ENGINEER will be considered new Pro/PDM objects when submitted back to a Pro/PDM database.
Part Mode:
*Why aren't part files saved when File, Save is selected in Sketcher?
While in Sketcher, the File, Save functionality will save the section to disk rather than the part file. This functionality allows sections to be stored to disk for future use in feature creation. Section files are saved to disk with a .sec file extension. Once Sketcher is exited by either completing the feature creation or quitting, File, Save will save the part file to disk.
All family table instance information is stored within the generic model. Pro/ENGINEER does not save a unique object file to disk for each instance.
The File, Save As functionality allows copies of part files to be created using the following technique:
Select File, Save As. Pro/ENGINEER will open a Save As dialog box. The current object in memory will be the default object to copy (in the Model Name section of the dialog). The name of the new object is specified in the New Name line in the dialog.
Assembly Mode:
*Does Pro/ENGINEER save all components each time an assembly is saved?
By default, Pro/ENGINEER does not store all assembly components to disk upon each File, Save operation. Instead, Pro/ENGINEER will save the assembly file and only components that have been modified. By setting the config.pro option "save_objects", this can be changed. By using this option, Pro/ENGINEER can be instructed to save all dependent objects, save only the objects that were modified, or save modified objects and objects specified by the user.
By default, Pro/ENGINEER will store objects that are assembled from other directories back to the directory of origin. If the user does not have write access to the directory, Pro/ENGINEER will not store the objects in the current working directory, unless specific config.pro options have been set. The config.pro options "override_store_back" and "save_object_in_current" allow greater control over this type of situation.
By default, Pro/ENGINEER will only store modified objects and will always store objects back to the directory from which they were retrieved. Therefore, if a part from a write protected directory has been modified and File, Save is selected, Pro/ENGINEER will not be able to save the object unless the config.pro options "override_store_back" and "save_object_in_current" are utilized.
During assembly creation, it is possible to add components to
the assembly that are located in directories other than the current working
directory. When the assembly is saved, the assembly file is saved to the
current working directory while modified components are saved back to the
directories of origin. If the assembly is cleared from workstation memory
by either exiting Pro/ENGINEER or by selecting File, Erase, and
selecting all the objects in the ERASE dialog box and then retrieved, it
is possible that Pro/ENGINEER will not be able to locate certain components.
The config.pro option "search_path" can be used to specify directories
which Pro/ENGINEER will search for objects. The config.pro file must contain
a separate "search_path" option for each directory to be searched.
Refer to the Configuration Options section of the Pro/HELP for
details.
*How does File, Save As function in Assembly mode?
In Assembly mode, the File, Save As functionality allows any or all members of the assembly to be copied.
By default, after selecting File, Save As, a dialog box will appear with the name of the assembly to be copied specified next to Model Name. The new assembly name is specified on the next line (New Name). After selecting OK, a check mark can then be placed next to each assembly component to be copied or Include all subcomponents can be selected to copy all assembly components.
If a check mark is placed next to any of the components or if Include all subcomponents is selected, Pro/TABLE will be displayed where new component names can be specified in the cell adjacent to the original.
If OK is selected without selecting a component or Include all subcomponents, Pro/ENGINEER will create only a copy of the assembly which references the original components.
The config.pro option "model_rename_template" is used to create a user defined renaming scheme.
Refer to the Configuration Options section of the Pro/HELP
for further information.
*Why do parts intersected by assembly features require renaming
before they can be stored?
Assembly features which intersect assembly components alter the
geometrical intent of the original object. When the assembly is in session,
the component exists in memory in two different states. When Pro/ENGINEER
tries to save the assembly, it is unclear which state of the component
is to be saved. Pro/ENGINEER will prompt the user to save the object with
a new name. This will create a copy of the object containing the geometric
result of the assembly feature.
If the config.pro option "override_store_back" is set to "yes", Pro/ENGINEER will save objects retrieved from other directories to the current working directory;
If "override_store_back" is set to "no", which is the default, objects will be saved in the directory of origin. If the option is set to "no" and the user does not have write access to the directory of origin, Pro/ENGINEER utilizes the config.pro option "save_object_in_current".
When the config.pro option "save_object_in_current" is set to "yes", Pro/ENGINEER will save objects to the current working directory if the user does not have write access to the directory from which the object was originally retrieved. If the option is set to "no", Pro/ENGINEER will not save the object at all. This option should be used in conjunction with the config.pro option "override_store_back".
The File, Save As functionality is the best way of copying assemblies.
The following procedure should be used to rename assembly components:
Drawing Mode:
*What is the preferred method to rename a drawing?
The File, Rename functionality should be utilized to rename a drawing.
The following procedure should be used to create a copy of a Pro/ENGINEER
drawing:
The default model orientation can be redefined by setting the config.pro options "x_angle" and "y_angle" to the desired values of the rotation, in degrees, of the object about the x and y axis. In addition, the model can be saved in user defined orientations by selecting View, Saved Views, entering a unique view name, and then Save. The model can easily be reoriented into the saved view orientation by selecting View, Saved Views, selecting the saved view name and then Set.
No configuration is required within Pro/ENGINEER in order for a spaceball to be recognized. If Pro/ENGINEER does not respond to the spaceball, we recommend contacting your systems administrator or hardware vendor for diagnostics.
Shading:
*How can the quality of a shaded model be increased?
The quality of the shaded model can be increased be selecting View, Model Display, Shade. Specify the shade quality between 1 and 10; the number 3 is the default. Increasing the shade quality to higher values may result in an increase in shading time. In addition, Small surfaces may be check marked in order to shade very small surfaces, such as round features, which otherwise may not be shaded unless the model is zoomed in.
Pro/ENGINEER shaded models will revert to wireframe if the machine is not configured for hardware shading capabilities. In order to have the model remain shaded during a spin operation, the workstation must have an appropriate graphics card installed, and the "graphics" option in the config.pro file must be set based on the type of workstation being used. Refer to the Hardware Configuration Notes on www.ptc.com for specific details.
To create an encapsulated postscript (EPS) file of a shaded model select File, Export, Image, change the type to EPS, and then OK. Select Dimensions Size, or Resolution DPI or Image Depth for additional options and finish by selecting OK.
Refer to the Hardware Configuration Notes on www.ptc.com for details on EPS plotter support.
When the config.pro option "shade_surface_feat" is set to "no", surface features will not be displayed when the model is shaded.
Colors:
*How is a color map file stored to disk?
A user defined color map can be stored to disk by selecting View, Model Setup, Color Appearances, File, Save As, and enter the name color.map in the New Name field in the Save As dialog box. Pro/ENGINEER will create a file called color.map in the current working directory.
The color map file, color.map, will be automatically loaded if it is located in the directory that Pro/ENGINEER is executed from. The configuration file option "pro_colormap_path" can be used to specify the location of a color map file that is not located in the startup directory.
The exact number of colors that can be defined will vary, depending on the type of workstation and the graphics card that is being used. Higher end graphics cards will typically allow a greater number of colors to be defined.
The transparency functionality is offered only with hardware graphics configurations. Refer to the Hardware Configuration Notes for other items available with hardware graphics configurations.
On machines configured to use hardware graphics, the transparency functionality must be enabled by selecting View, Model Display, Shade, and Enable the Transparency option.
Colors assigned to parts in Assembly mode do not effect Part mode. This functionality allows assembly colors to represent a production operation done after assembling the individual parts, e.g., the application of paint.
Colors applied to components in Assembly mode will override colors defined at the Part level. To unset an assembly color, retrieve the assembly and select View, Model Setup, Color Appearances, Component, select the component in question and then Unset.
Exploded Views:
*Why does a subassembly explode when the top-level assembly is exploded?
By default, subassemblies explode when the top-level assembly is exploded. The top-level assembly can be modified to specify which subassemblies and which parts within the subassembly to explode by selecting Modify, Mod Expld, Expld Status. Select Toggle Expld from the EXPLD STATUS menu and pick the components in the Model Tree that are not to be exploded (changing the value to Unexploded).
This functionality is not currently implemented in Pro/ENGINEER. However, datum axes can be created using one of several available methods. The type of datum axis to use will depend on the specific situation.
Exploded views can be saved to a name by exploding the assembly, then selecting View, Saved Views, and then Save a new name. When an exploded view name is retrieved, the assembly can be unexploded using View, Unexplode.
The File, Working Directory menu selection allows the Pro/ENGINEER working directory to be changed. After selecting Working Directory, Pro/ENGINEER allows navigation through the directory tree structure.
When Window, Open System is selected, Pro/ENGINEER will execute a system shell. The current working directory for this shell is the Pro/ENGINEER working directory. The Pro/ENGINEER session will be suspended while the system window is active. Exiting out of the system window will allow the Pro/ENGINEER session to continue.
The Pro/ENGINEER session will be suspended while the system window is active. Exiting out of the system window will allow the Pro/ENGINEER session to continue.
The Technical Support Info menu ('Customer Services Info' in earlier versions) selection will open
a Pro/ENGINEER information window giving the active Pro/ENGINEER config
ID number, the Revision and build of Pro/ENGINEER, and almost all information
about your system's configuration. This information is specific to your
site and used by Parametric Technology Technical Support as a means of
determining your software configuration and licensing.
The Technical Support Info menu selection will open a Pro/ENGINEER
information window providing the following information:
• Software Version
• Configuration Id
• Pro/ENGINEER loadpoint directory
• License Configuration (Locked or Floating)
• All included Pro/ENGINEER options
• Machine Information
• Hostname
• Username
• CPU id
• Machine type, OS name, release, and version
• Pro/ENGINEER graphics type
• Installation Directories and Command Information
• Configuration Information - Configuration files read
• Auxiliary Application Information (includes floating option information
if available)
This information is specific to your site and used by Parametric Technology Technical Support as a means of determining your software configuration and licensing.
It is written to a support.inf file in the current working directory of Pro/ENGINEER.
The Utilities, Mapkey menu selection is used to create a mapkey by recording a series of menu picks and assigning these picks to a keyboard key or keys. The created mapkey can be stored in the config.pro file for use in other sessions of Pro/ENGINEER or be specified to be used in the current session only.
When Utilities, Mapkey is selected the Mapkey dialog box
appears with the following options.
New - Create a new mapkey and starting recording picks.
Modify - Modify the highlighted mapkey.
Run - Execute the highlighted mapkey.
Delete - Delete the highlighted mapkey.
Save - Save the current mapkeys to a config.pro file.
See the Suggested
Technique for Creating Mapkeys using the Mapkey Functionality for more
information on the Mapkey functionality.
Trail Files:
*In which directory does Pro/ENGINEER create trail files?
Each time Pro/ENGINEER is executed, a trail file is created called trail.txt.n; where n represents the file version number which monotonically increases with each new file. By default, Pro/ENGINEER trail files are written to the current working directory. The config.pro option "trail_dir" can be used to specify a directory to which the Pro/ENGINEER trail files are to be written.
Pro/ENGINEER does not allow trail files to be executed having the file name "trail.txt". The file must be renamed since Pro/ENGINEER creates a new file "trail.txt" each time the software is executed. Trail files must be in the format filename.txt; where filename represents a string other than "trail".
There are many possibilities that would lead to a trail file going out of sequence. Before executing the trail file, the Pro/ENGINEER environment must be exactly the same as it was during initial creation of the trail file. For example, if the trail file retrieves a part and makes modifications to it, the same version of the part must reside in the same location as it was found initially. In addition, the same config.pro options must be utilized. If, for example, the display of datum planes was modified, this could cause an out of sequence error. If a trail file does go out of sequence, the user will be notified of the line number that could not be executed. To troubleshoot this type of problem, copy the original trail file to a backup name, then edit the original trail file by removing all the lines after the one that caused the out of sequence error. Also remove five to seven lines before the point of failure. At this point, rerun the edited trail file, then manually walk through the menu selections by viewing the backup trail file. By doing this, it will be clear what is causing the problem.
With the config.pro option "set_trail_single_step" set to "yes", a trail file will stop after each trail file step. Entering a carriage return will allow the trail file to proceed.
The config.pro option "trail_delay" will force a trail file to pause for a specified number of seconds between trail file steps. The value for the "trail_delay" option is the delay period specified in seconds.
The default size of the Pro/ENGINEER working window can be controlled using the config.pro option "windows_scale". The window scaling factor is specified as the value to the "windows_scale" option ranging from 0.5 to 1.0. The default value for the "windows_scale" option is 1.0.
Pro/ENGINEER must be restarted in order for modifications to the value of "windows_scale" to appear.
There are several config.pro options that can be used to change the Pro/ENGINEER menu fonts.
The configuration file option "default_font" option is used to change the font used by Pro/ENGINEER for items other than the menu bar, menus and their children, and pop-up menus. For Unix machines, this must be the name of a font available at the X-server running Pro/ENGINEER. The "xlsfonts" command can be used to list available system fonts. The standard default font for Unix systems is helvetica, regular,12. The standard fonts for Windows NT and Windows 95 are inherited from the system settings made with the Control Panel. The "default_font" format should be:
default_font name, style, point_size
Spaces are acceptable and the values may be in any order. Example:
default_font courier, italic, 12
In addition, the configuration file options "menu_font" and "popuphelp_font" can be used to separately control the font of the menus and pop-up screens. Pro/ENGINEER must be restarted in order for these modifications to appear.
Pro/ENGINEER does not currently allow the default location of the Pro/ENGINEER working window to be redefined, however the scale of the working window can be modified using the config.pro option "windows_scale".
With the config.pro option "menu_horizontal_hint" set to "right", Pro/ENGINEER will place the second column of menus to the right of the primary menus i.e. the ENVIRONMENT menu will appear to the right of the MAIN menu instead of overlapping the Pro/ENGINEER working window. Be aware that the working window may require a scaling factor using the config.pro option "windows_scale" to provide ample screen space for the secondary menus to be displayed.
Pro/ENGINEER must be restarted in order for modifications to the value of "menu_horizontal_hint" to appear.
With the config.pro option "iconify_entire_pro" set to "no", individual working windows can be iconified. The default value for "iconify_entire_pro" is "yes".
The mapkey functionality allows a series of Pro/ENGINEER menu selections and keyboard input to be executed by a keyboard command. If a mapkey will not execute properly, check the following:
The mapkey functionality is documented in the Pro/HELP Online Documentation, under the topic To Define Your Own Mapkeys.
All lines in config.pro are limited to 80 characters. Mapkeys
containing many characters may be nested together to define a single operation:
Refer to the Pro/HELP Online documentation for further information.
The display of datum planes is a toggle function in Pro/ENGINEER.
One mapkey is used to toggle the display:
MAPKEY dtm #ENVIRONMENT; #Disp DtmPl
Or, as of Release 20, there is a Toolbar icon which can be unselected for
each of the datum features.
Only the first mapkey defined in config.sup will be recognized in Pro/ENGINEER, per the definition of config.sup.
Function keys may be used for mapkeys and should be defined as
follows:
MAPKEY $F2 #FEATURE, #CREATE, #COSMETIC, #SKETCH, #NO XHATCH, #DONE
The "$" sign tells Pro/ENGINEER that F2 is the function key "F2" and not
the alpha-numeric characters "F" "2". For NT machines, F10 is predefined
as an NT utility and cannot be defined for a mapkey. For more information
refer to the Pro/HELP Online Documentation.
A mapkey may execute another mapkey. This is called nesting mapkeys:
MAPKEY param #set up; #parameters;
MAPKEY string %param; #part; #create; #string;
This example has the first mapkey "param" making the menu selections
to shade the model. The second mapkey "string"
executes the first mapkey "param", defined by %param, and then creates
a string parameter. For more information refer to the Pro/HELP Online
Documentation.
*How can keyboard input be included in a mapkey?
Keyboard input can be entered during the execution of a mapkey by selecting Pause for Keyboard Input during the mapkey creation. Then, when making the menu selections that will be included in the mapkey, Pause must be selected to allow the mapkey to stop, so that keyboard input may be entered. For example, to create a mapkey that will automatically create a new part, with a user-defined name, consisting of a default set of datum planes, refer to the Suggested Technique for Creating Mapkeys using the Mapkey Functionality . In this case, the mapkey would pause and wait for the user to input the name of the model, then continue on after the user presses the Resume button to create the default datum planes.
A mapkey may prompt for a screen pick, however it cannot continue once the selection has been made. An alternative technique is to define a second mapkey which will continue once the screen selection has been made.
Detailed documentation can be located in the Suggested Technique for Customizing Pro/ENGINEER menus using menu_def.pro .
Similar to config.pro, menu_def.pro file can reside in any of 3 directories.
The default Pro/ENGINEER menu selections may not be modified or removed.
If the added menu selection aborts prematurely, check the following:
All menu_def.pro menu additions will be displayed in the bottom of the target menu.
A menu_def.pro will not allow a new menu to be created. Only new menu selections can be added to existing menus.
To change the name of a feature, select Set Up, Name, Feature, select the feature, then enter the new name for the feature. To modify dimensions, select Modify, Dim Cosmetics, Symbol, then enter in the symbol to replace the dimension symbol, "d#".
There is no limit to the number of rows and/or columns that can be included in a family table. The size of the dialog box may have to be expanded, in order to see a large number of rows and/or columns at one time.
In order to enter negative values, the dimension symbol must be preceded by a "$" sign when added to the family table.
Nested instances refer to instances created within other instances.
A .ptd file is a text file containing all the information found in the family table, including all instance names and their current values. The .ptd file is created by selecting File, Export Table, and selecting Pro/TABLE as the type of file to export. This file is not required for part retrieval and can be deleted. However, the .ptd file can be used to edit the family table outside of Pro/ENGINEER. If an instance is deleted by modifying the .ptd file, subsequent retrieval of the generic will ask the user if he or she wishes to clean up the family table, at which point any modifications made to the .ptd file will be reflected in the internal family table. In addition, as soon as the generic is stored, the internally stored family table will take precedence over the local .ptd file, if one exists in the current directory. When a generic part is retrieved in a directory where an external .ptd file resides, the external file will take precedence over the internally stored family table. The name of the ptd file will always have the same prefix as the name of the generic part. The .idx file is an instance index file and contains a list of all current instances within a directory. During object retrieval using File, Open, all instances will be listed in the menu structure if the .idx file is present in the current working directory. The default name of all instance index files will be {directory_name}.idx.
If a regeneration failure is encountered during verification of one of the instances, retrieve the generic part and modify the dimensions of the generic to those of the instance that failed. At that point, the reason for the regeneration failure of the instance can be determined.
To prevent all instances from showing in the Pro/ENGINEER menu structure, delete the instance index file, or set "menu_show_instances" to "no" in config.pro.
To add an instance as a drawing model, the instance must be specified from the directory tree, either by using the .idx file or using the In Session button.
When a feature is created on an instance, the new feature is automatically placed in the family table and will be suppressed in the generic and all other instances.
In order to replace assembly components using an assembly family table, enter the name of the part instance in the family table cell, instead of entering Y or N.
To control part features and dimensions from an assembly family table:
When a feature is created in Pro/ENGINEER, dimensional and geometric references are created. These references, whether they are edges, surfaces, or vertices, will belong to other features that already exist on the model. When such a reference is established, this is referred to as a parent-child relation. The newly created feature is now considered a child of any feature that contains an entity that was used as a reference.
Yes, a feature can have more than one parent. For example, if a cut is created in such a way that the sketching plane chosen was a surface on the base feature and then the cross section of the cut has a dimension that defines a distance from a datum plane, both the datum plane and the base feature are considered parents of the cut.
Yes, a feature can have more than one child. It is not uncommon for the first feature of a model to have dozens of children. For example, if a default set of datum planes is the first set of features created on a model, all subsequent geometry will be children of one or more of these datum planes. The initial feature will typically use two of the datum planes for references, one as a sketching plane and one as vertical or horizontal reference. In addition, any feature that uses this newly created feature as a reference will now become a child of the the datum planes that are the parents of the first feature.
If a feature containing children is selected to be deleted or suppressed, Pro/ENGINEER will highlight the child in blue and ask for an action to be taken. Without the parent, the child will not have a complete set of references and will not be able to regenerate. Therefore, when attempting to delete or suppress a parent, the child must be rerouted, deleted (or suppressed), or suspended. These options will be listed in the CHILD menu, which will appear automatically when attempting to delete or suppress a feature with children.
In order to obtain a complete list of parents or children of a particular feature, select Info, Parent/Child. At that point, a prompt will appear asking if information on parents or children is desired. Once this selection is made, select the desired feature, and the information will be displayed.
Pro/TABLE is a stand-alone program that can be invoked without
using Pro/ENGINEER. To execute a session of Pro/TABLE from a command line,
type in the command "protab". This allows some tables, such as sheetmetal
bend tables, to be edited outside of Pro/ENGINEER.
The width of a Pro/TABLE column can be changed by selecting Format from the Pro/TABLE menu. All of the columns can be changed by selecting Global Width, or some of the columns can be changed by selecting Column Width and highlighting the desired cells. In order to reset the column width back to the default value, select Format, Reset Width.
After utilizing a session of Pro/TABLE, the size of the buffer used to write data to the trail file will increase. If the trail files are being written across an NFS mount, i.e., if the Pro/ENGINEER startup directory is a shared file system that has been mounted across the network, there may be a noticeable decrease in system speed. To solve this, set the config.pro option "trail_dir" to a directory that is local to the Pro/ENGINEER client machine.
There is no limit as to the number of columns and rows that can
be used in Pro/TABLE.
Pro/MECHANICA Motion requires to install a Microsoft C compiler on your system.
Most likely you just forgot to set the MM_C_HOME environment variable after the installation.
In order to avoid an unnecessary slowdown of your machine, wasted harddisk space etc. users of other
C-compilers or users which do not program C at all might want to copy the "bin", "lib" and "include"
directories from a colleague having a complete installation.
Don't forget to order/register your copy at DISTRILOG, as each license must be registered with the SIC.
Example (using the MS Visual C++ default path; include in autoexec.bat):
SET MM_C_HOME="C:\Program Files\Microsoft Visual Studio\VC98"
(Under WinNT/2000 you might want to use the "Environment Variables" dialog)
A possible reason - besides a missing license - is a misconfigured environment variable.
You need to set or correct MECH_HOME which contains the path to your Pro/MECHANICA executable.
Example (include in autoexec.bat):
SET MECH_HOME=D:\promech2000i2\i486_nt
(Under WinNT/2000 you might want to use the "Environment Variables" dialog)
[parts of the faq are (C) PTC]