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Mirroring RH Models to become LH Models in Intralink

Hacks

New member
Guru's,



I have searched PTC's knowledge base and here at ProECentral and know how to mirror a part or subassembly model from a RH configuration in order to get the LH configuration.



What I'm not sure of is how to go about this with the model and their associated drawings in the Intralink environment.



Specifically, how can you mirror a RH model that has an associated drawing in a workspace to get the LH model and drawing? Would Duplicate Objects come into play at some point? Has anyone come across this dilemma before and developed a methodology to resolve it?



TIA,

Brad Hacker

ME CAD Admin

Zebra Technologies Corp.
 

jabbadeus

New member
I would create the mirror in Pro E, save the drawing under a different file name, then replace the mirrored part in the drawing for the original.



To create the mirrored model:

1. Create a dummy assembly.

2. Assemble the original to the default constraint.

3. Insert > Component > Create > Part > Mirror. (That's WF; for 2001, replace Insert with Assembly.)

3. Select the original as the part reference. Select a part surface or datum-- NOT an assembly datum-- as the mirror reference.

4. Save the new part.



To copy the drawing:

1. Open the original.

2. File > Save A Copy.

3. File > Properties > Drawing Models > Replace Model.



You may have to do some cleanup work on the drawing, moving views and details around. Sorry I don't know if there's an Intralink solution.



Dave Martin
 

Hacks

New member
Thanks for the reply Dave.



Everything was working fine until I got to the Replace pick underneath the Views -> Dwg Models.



when I open the drawing and go to replace the model, I get the following message:



The drawing's model is unchanged.



I then tried added the new mirrored model to the drawing and was able to set it as current. However, when I went to replace the model in the drawing, the following message appeared:



No model in the drawing has a family for replacement.



I'm trying to complete your steps in order to ascertain how much drawing clean-up work would be required.



Any ideas on what I'm doing wrong?



Brad
 

jabbadeus

New member
Darn it, brain fart by me. That's right, Replace Model is only for family table members. Sorry. Let me think if there's another way to use the same drawing instead of recreating it from scratch...
 

cristelino

New member
You have two different cases



In my opinion do something like:

1 Create a new Datum plane ( but only if the simetry plane can be outside the model,is the first case)

2 create Mirror>all feat

3Create Cut > and eliminate features mirrored>save as

4 remove ``all not displayed``



In the second case you can use :Feature operation>copy with move>all feat and try ``cylindrical``



Cristian
 

CJ

New member
Here's a slightly long winded solution to your problem.



Follow steps 1-4 in jabbadeus's reply



export the RH drawing & model to a folder.

open this drawing in a non Intralink linked ProE session

rename both drawing & model in session & on disk,through ProE, to the new LH model number.

Import the renamed drawing only into Intralink, It will look a the original LH model in Intralink when it is opened.



It should work I have used this method many times.
 

Hacks

New member
Thanks CJ, your suggestion worked with one, minor change I had to perform.



Importing the drawing file did not work - it gave me the same RH model in the drawing. However, launching a session of Pro linked to a WS and navigating to and opening the drawing file does show the new LH version of the part in the drawing. Some drawing clean-up is required with dimensions but this process is a lot quicker than re-modeling the mirror image of a part feature-by-feature.



A couple other comments:



Not all sheetmetal features can be mirrored if you select Copy as the Type in the Mirror part dialog box. Using Reference for the Type will allow for a mirror of all features to occur but there's obviously a p/c relationship that is created with the source part (which may be undesirable depending on your design intent) and the only item in the Model Tree is a Merge feature which you can't redefine. As a matter of fact, you can't do much at all with it.



After doing the mirror/copy, all the user defined model parameters became undesignated in the model file. Not a big deal to re-designate but annoying.



Lastly, I had to replace the drawing format as it lost the smarts we give it for grabbing Intralink system attributes (like revision and version) once it was exported from the WS. Again, not a big deal.



Thanks again for everyones help.



Brad
 

Hacks

New member
Ran across another problem that I've seen before but, of course, did not see with the two part and drawing combo's I tested this out on (Murphy's at it again!).



How does one get around this message so one can rename an item outside of Intralink?



View attachment 348





The two part/drawing files I did test this on were not sheetmetal parts - the one causing the message above is.



Wouldn't think that has anything to do with it but I seen stranger stuff with Pro.



Once again, any help would be greatly appreciated.



Brad
 

Hacks

New member
Maybe I should investigate a little more before posting.



I think I figured this out by playing around with two config.pro options.



let_proe_rename_pdm_objects (yes or no)

rename_drawings_with_object (none, part, assem or both)



Could fix the problem by enabling the let_proe_ rename... option but I don't want folks renaming in Pro. That should be done in the Intralink environment.



Instead of using a rename, I'm going to use Save a Copy... with rename_drawings_with_object set to both. This will automatically copy the drawing to the new name when saving a copy of the part file to the new name provided the drawings original name was the same as the part files original name and is residing in the same location as the part file.



Brad
 

bhayden

New member
You found the config-pro option around the warning but I would not recommend that you use it. If you ever make a mistake and corrupt the Intralink (Oracle) database you're going to be hating life. It's usually easier to rename the parts in Intralink from the Common Space browser. If you need to a Sync with Common Space will then update workspace copies. If parts are not checked in yet to the Common Space you can rename them in the Workspace. These are all things to keep you from hurting yourself!



-Bernie-
 

Hacks

New member
Thanks Bernie, I understand what you are saying and couldn't agree with you more.



However, as I indicated earlier, I'm not going use the let_proe_rename... option but do plan to use the rename_drawings... option OUTSIDE of the Intralink environment.



Brad
 

CJ

New member
If you import the drawing to be renamed into a new workspace it will show as same name already exists, but intralink will let you rename it to the new number & maintain the link to the drawing.



CJ
 

Hacks

New member
I moved onto to trying to do this with subassemblies (i.e., a sheetmetal part with PEM fasteners) and there are several extra steps to perform and some extra baggage to go along for the ride but we still find value in it if I can just get past this one issue that just kills it for us.



I can't get the views in the newly created opposite hand drawing to come in as mirror images of their counterpart views on the opposite hand drawing. The main view is coming in as a 3D view and not as an orthographic projection. Of course this messes up the other views projected off of this view and the dims so as magenta as a result of this. Setting the main view to the mirror of its counterpart corrects the view issues on the drawing but the dimensions get blown away and all the views have to be re-dimensioned.



I saw this view issue happen when I was initially investigating doing this with part models and can't remember what I did to correct it. In this case, I thought it might have been related to the fact that the first subassembly part I tried this on was a true sheetmetal part using PEMs but that wasn't it as a ordinary solid part with PEMs in it exhibited the same problem.



Any ideas on what's happening?



Thanks,

Brad
 

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