Save an assembly relationship by replacing one part

[atomic.lex]

Hi there,

I've been trying to save an assembly relationship by C one part with another. Both parts are not the same and they have some different compositions. I have an idea, what it could be possable to save a relationship by using the same name for different axis. But it doesn't work. Have you any suggestions???

Much success

Atomic Z

[atomic.lex]

Hi there,

I've been trying to save an assembly relationship by C one part with another. Both parts are not the same and they have some different compositions. I have an idea, what it could be possable to save a relationship by using the same name for different axis. But it doesn't work. Have you any suggestions???

Much success

Atomic Z

[YannickEnrico]

Every line, vertex and face has a new ID in Inventor. 

If you want to replace and keep the relationship, you'll have to save another version of the original part, and then change the dimensions you want to change. 

Alternatively I -think- if you constrain using only the original planes, it'll work out. 

[SBix26]

It is possible to save a Constraint relationship (probably similar for a Joint relationship).  When you replace the component with one that is not a direct copy, the relationships will break.  Simply right click on the broken relationship in the browser and select Edit.  The selection button for the missing side of the relationship will already be selected, all you need to do is pick the new component feature to complete the constraint and then click OK.

Hope that helps,

Sam B

Inventor Professional 2018.1.2
Vault Workgroup 2018.0
Windows 7 Enterprise 64-bit, SP1

[SBix26]

Here's my reply in your duplicate thread:

It is possible to save a Constraint relationship (probably similar for a Joint relationship).  When you replace the component with one that is not a direct copy, the relationships will break.  Simply right click on the broken relationship in the browser and select Edit.  The selection button for the missing side of the relationship will already be selected, all you need to do is pick the new component feature to complete the constraint and then click OK.

Hope that helps,

Sam B

Inventor Professional 2018.1.2
Vault Workgroup 2018.0
Windows 7 Enterprise 64-bit, SP1

[kelly.young · Accepted solution]

Hello @atomic.lex if the parts are referencing the Derived surface of the master part, when you replace them if setup correctly they should replace to the same location.

Another way if you take your 1st part, save as, then add or edit the newly created 2nd part, if the constraint location is the same and not deleted or broken, ie. the face plane or concentric center, it should stick.

You could also create iMates to locate the parts.

Please select the Accept as Solution button if a post solves your issue or answers your question.

[johnsonshiue]

Hi Kelly,

The derive case you are talking about is limited to replacing derive part A with derive part B, while the two derive parts have the same source part. If you replace the source part with its derive part or vice versa, the constraint will still fail.

It is true that iMate can help mitigate the limitation. It is because iMates match by type or name. As long as the new part has the same iMate type or name, the constraint will survive after component replacement.

Many thanks!

[rmcdougallLXU26]

This is a really unfortunate limitation with Inventor. If I have a part within an assembly and the part has a whole bunch of relationships, it's extremely time consuming to repair all the relationships upon replacing it with. Even if I replace the part file with an assembly file containing ONLY the exact same base part file, oriented identically, all relationships fail. Other CAD platforms do not have this issue (ie Solid Edge).  Is there any other workarounds?

[CGBenner]

@rmcdougallLXU26 

Welcome to the forum.

This situation may depend greatly on what is being replaced, and with what.  It might help if you could provide some small examples such as an assembly in two forms:  First with the original part fully constrained how you want it.  Second with the part you want to replace it with, and showing the resulting constraint failure.  That would give the experts here something to look at and hopefully offer some advice.  Good luck!

[rmcdougallLXU26]

@CGBenner maybe this series of screenshots will help. From experience, Solid Edge would accommodate this 'replace component' workflow with no issues but Inventor can't handle it, very disappointing. Running Inventor Professional 2023 BTW (if it matters). The larger the assembly, the greater the impact (depending on which component is being replace and how many constraints it has). 

1. Top level assy2. Child part file3. New child subassy file, containing only the part file4. Result after trying to replace part file with subassy file in top level assy

[johnsonshiue]

Hi! The assembly constraints will survive after replacement only if the new part shares the same document ID with the old part. Also the geometry has to be similar. If possible, please share an example illustrating the issue with me directly johnson.shiue@autodesk.com. I would like to take a look to see why the constraints did not survive after replacement.

Many thanks!

[atomic.lex]

Hi!
Back to my post 7 year ago: I've escaped those "lost'n'repair" problems due relations only with points, axis and sides of Origin. 

[rmcdougallLXU26]

@johnsonshiue I should have posted with a clarification initially. I'm able to replace part for part, assuming I just re-name the original part and replace it with the re-named version. The errors I'm seeing are happening when I try and replace a part with an 'equivalent' assembly. I'm sure you could replicate this error that I've shown above with any old parts you had on hand. The constraints always fail upon replacing with an 'equivalent' assembly, and this makes sense if it's relying on document ID to be equivalent - but that doesn't make it OK. It's fairly standard workflow for me (and I imagine others) to replace a part with a subassembly. Competitive platforms support this. Is there a way to submit this as an enhancement request? 

[johnsonshiue]

Hi! Please feel free to submit an enhancement request to Inventor Ideas. However, this has been treated as a limitation for a quite while.

Many thanks!

[emanuel.c]

I would looove for this to be better implemented! I didn't know SolidWorks or others do this better - have used it way too far back. I often replace parts with assemblies or with other parts and it would be sooo much easier if it would remain constrained and properly. Though I assume it's easier said than done.

But... just like mirroring in assemblies in Inventor (an absolute no go for me) it becomes something you unfortunately get used to...