The following are configuration file options that relate specifically to large assembly drawings. Making use of these options can significantly improve drawing productivity.
Assembly Manipulation Techniques
The following suggestions can be used in Assembly mode prior to Drawing creation:
Create the simplified reps you need for the drawing.
Don't mix up several simplified reps in one drawing because you'll have to load all parts again.
If its necessary to have several representations in one drawing, create first for each rep one drawing and merge them later together to a multiple sheet drawing.
Use Simplified Representations to prevent Pro/ENGINEER from retrieving unnecessary models into memory.
Replace models that are not referenced in a drawing view with Geometry Reps. Geometry Reps take approximately half the time to retrieve as the master model.
Use as few assembly features as possible because intersecting components creates hidden copies of the model and this uses additional memory. When sketching assembly features, use closed sections and manually select the components to be intersected. This will prevent Pro/ENGINEER from intersecting extraneous components and will speed up drawing performance.
Increasing Performance when Working with Large Assembly Drawings
The following methodologies can be utilized in drawing mode to increase drawing productivity:
Set the line display of all views to Wireframe. Regeneration time will be faster than if the display of the views are set to Hidden or No Hidden.
Erase views that are not being used when detailing the drawing. By erasing a view the display will not be calculated by Pro/ENGINEER and this will decrease regeneration time. Use Views, Resume View to resume the views before plotting.
Move views, which are complete to separate sheets of the drawing. The views can be moved back to the original sheet prior to plotting.
Use Z-Clipping to reduce graphical information displayed in an assembly view. All geometry behind the Z-Clipping plane will be removed from the display.
Use Views, Dwg Models, Add Model for adding subassemblies to the drawing. Create views of the subassemblies instead of creating views of simplified representations of the master assembly.
Create separate drawings whenever possible, as this will prevent Pro/ENGINEER from retrieving unnecessary models into memory.
Use Pro/BATCH so all plotting can be performed outside of Pro/ENGINEER
To minimize retrieval time when plotting, use View Only retrieve. The config.pro option "save_display" must be set to "yes" prior to saving the drawing.
The display of components in an assembly can be blanked in a drawing. Create layers to blank the display of many components in an assembly. Use Views, Disp Mode, Memb Disp and Blank to also blank the display of assembly components.
When working in a drawing and changing the part (or assembly), all views of the drawing are unregenerated. After switching back to the drawing, all views of the current sheet are regenerated automatically. This could last up to 1 hour and more.
By setting the config option auto_regen_views to no, the views are not regenerated automatically. So the user has control using Views - Regenerate View to regenerate the view, which he currently needs to go ahead with his work (Often the user is doing a change in the model and he needs only one view to be updated at the moment).
Exception: When changing display of a layer, the views are regenerated regardless of this option setting. PTC development is working on this problem.
If it hurts too much, use these workarounds:
If you find a better solution, please inform me.
To speed up working in drawings you can
When retrieving a drawing, ProE needs time for following steps:
Retrieval of drawingfile and all
modelfiles, then the display of all views has to be regenerated. When the drawing
has several sheets, then the views of the sheet, which was current when saving
the drawing, are regenerated.
This regeneration of the views takes most of the time, when retrieving a drawing.
Example cylinderheaddrawing: Load of files takes 1 min., regeneration of views
takes 20 min.
To speed up retrieval time, you can either
The config.pro option FORCE_WIREFRAME_IN_DRAWINGS is probably too confusing for working with complex models.
Everybody should be aware, that all views should be regenerated before plotting.
The option CREATE_DRAWING_DIMS_ONLY should be set to yes. If you don’t do this, the dimensions, which you create in your drawing will be saved in the .prt file. If you create a drawing with created dimensions and you forget to save the model as well you will loose all the created dimensions.
If you work parallel with y
our model and the drawing in different windows you shouldn’t modify you environment settings. If you do this all views will be regenerated. A workaround is to set the fast hlr option. Another way to avoid long waiting times is to modify the display mode of the different views separately by using the DISP MODE, DISP VIEW command.
The command VIEWONLY RET can save a lot of time during the retrieval of a drawing. But if you did not regenerated all views before you saved the drawing, you’ll see at the next retrieval with this command only bounding boxes for the views which are not regenerated. The workaround is to create a mapkey which regenerates all views, saves the current drawing and quits Pro/E. Activate this mapkey in the evening before you leave.
If you set the SAVE_DISPLAY option to YES, you’ll get the views immediately if you retrieve a drawing. But be aware that this happens only to views, which have been regenerated before saving it. The rest will be regenerated. This causes sometimes nevertheless long waiting times.
Avoid regenerating. Do it before you go for lunch or at the end of the day before you leave.