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What replaces "master model merge" in Wildfire?

dr_gallup

Moderator
I'm getting along pretty well with wildchild but today I need to merge an existing part (a casting for instance) into a new part to make additional machining cuts. In the past I whipped out my handy master model merge cheat sheet, create an empty assembly but whoa, wildflower won't let me create the new part in the empty assembly. I'm sure there is some new functionality to do the same thing but I don't know what it is. I would like the exact same result as master model merge where there is no reference to the assembly
 

donha

New member
I think the route today would be Insert>Shared Data>Inheritance. I am not on Wildfire, but inheritance feature was introduced in 2001 to replace inserting the part into an assembly. Also, if you just assemble the part into an assembly and use assembly level features, you will achieve the same results.
 

Brian_Adkins

Moderator
I'd use an External Merge feature:

Insert / Shared Data / Merge From other Model



Inheritance features are cool, but they are a totally different approach to the MasterModelMerge method. Instead of getting a block of geometry, you get the entire model tree. You can also have dims and feature-existence different between the source and target models. This has good and bad points that you should evaluate before revising your process.



-Brian
 

dr_gallup

Moderator
In part or assembly mode I only see INSERT/SHARED DATA/FROM FILE.



I don't see Merge From other Model or Inheritance.
 

Brian_Adkins

Moderator
Ahhh....



Data-Sharing features are not available in Foundation... I think you have to have the Advaned Assembly Extension or something like that to get them...



In this case, you'll need to stick with the temporary assembly method of creating the merged models...



2001 : Component > Adv Utils > Merge

Wildfire 2.0 : Edit > Component Operations > Merge



-Brian
 

dr_gallup

Moderator
Ahhh....



I just realized that my Advanced Assembly Extension is not getting bound to the Foundation license when Pro/E is starting. So much for license simplification. I was able to get it fixed by running PTCSETUP. All better now, I see 6 more options in the SHARED DATA menu.



Thanks, everyone.
 

JONGPC

New member
dr_gallup:



I have the same problem......Advanced Assembly Extension not bound to Foundation. The IT dept. says that it's a licensing thing.......



Exactly what to do to get the problem resolved. I know we purchased the extension but it is not running.



Thanks,
 

dr_gallup

Moderator
You have to go to loadpoint/bin and run ptcsetup.bat. There is a point where you define startup commands and you have to attach available extensions to the basic license. I just created a new startup command (proe2.bat) that correctly attached the AAX extension.



You can read the license file with a text editor. You should see something like:



####### FLOATING License #######

# Serviceable = Pro/ENGINEER Advanced Assembly Extension



If you don't see that then you need to contact PTC licensing.
 

kvision

Moderator
You may merge them together as in previous versions using

edit>component operations> merge



So you can create an empty part with the welded or merged part number and merge the remaining parts into this empty part. This will generally produce the parts and part numbering needed.
 

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