Hi all
I am using INV 2012 and I wan to to know a trick how to convert the weldment assembly back to regular assembly template.
any macros are there please suggest me
Thans for advance.
Regards,
linus kotte
Solved! Go to Solution.
Solved by drawings. Go to Solution.
Hi linuskotte,
You can place the weldment in a new assembly, and promote (drag and drop in the browser) all of the components up to the top level and then delete the weldment assembly. Then simply save the new assembly as the correct part number to replace the original assembly.
But unfortunatly there is no button or option to turn a weldment assembly back to regular assembly.
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
I found that I can just copy parts from weldment to new assembly. By copying all relations are converted too.
Is there any way to do this with frame generator? When I try this with a frame generator part the frame is no longer associative to the skeleton sketch.
You can place the weldment in a new assembly, and promote (drag and drop in the browser) all of the components up to the top level and then delete the weldment assembly. Then simply save the new assembly as the correct part number to replace the original assembly.
Is there a way to do this without losing all mates to the weldment's origin?
Hi! Another option you can try is to demote all components from the weldment assembly to a new subassembly. The associativity should still remain. The subassembly should no longer be a weldment assembly.
Many thanks!
The actual solution is a combination of demoting and copy/paste feature. This is for Autodesk Inventor 2015.
I replied to the full thread as well, but here is the solution. It will move all your mates etc as well.
The actual solution is a combination of demoting and copy/paste feature. This is for Autodesk Inventor 2015, it may work with others as well.
@cdraghi3 wrote:I replied to the full thread as well, but here is the solution. It will move all your mates etc as well.
The actual solution is a combination of demoting and copy/paste feature. This is for Autodesk Inventor 2015, it may work with others as well.
- Open the weldment.
- Left click on the background and drag your cursor across the entire weldment assembly.
- This should highlight all the parts in the actual display.
- Right-click on the background, go to COMPONENT, then select DEMOTE.
- It will prompt you to accept the following: "Related assembly relationships moved with moving component(s)". You want to say YES to this or your constraints will not move with it.
- You will notice that inside your weldment, you now only have one item: an assembly of all the items that were just demoted.
- Now you need to right click on this assembly in the BROWSER and select COPY.
- OPEN a regular assembly file.
- Right-click and PASTE the assembly into the new assembly file.
- Now EXPAND this assembly.
- Select all the items within the assembly, click COMPONENT, and select PROMOTE.
- Again, it will prompt you to accept the following: "Related assembly relationships moved with moving component(s)". You want to say YES to this or your constraints will not move with it.
- You can now select the original assembly item that was copied from the weldment and DELETE it.
- Save this assembly!!
- You are done!
This still loses all mates to the origin planes/axes.
Hi! Are you using Inventor 2015 or earlier? If you are on newer releases, demoting components will preserve constraints between demote participants.
Many thanks!
I'm using 2019. Yes, constraints between components are preserved. The issue is I would like to be able to preserve mates to the origin axes/planes. Some assemblies have a lot of those.
I just did this (with a small assembly)
1. copy all parts
2. paste in new assembly
3. close original assembly
4. save new assembly OVER old assembly.
all constraints were preserved, and the parent assembly (of which the "old" assembly was a child) recalculated the constraints properly, when I opened it with the "new" assembly as the reference.
Using Inventor 2018.3
That technique didn't work for me, running 2019.1.2.
Was able to create new assembly, but no constraints were saved in the new assembly.
Had to recreate them.
Small assembly - 6 parts.
Hi! Could you share a bit more detail about the issue you are having? Did you try Demote? Select all components within the assembly and right-click -> Components -> Demote. Does it not work for you? Could you share the files here?
Many thanks!
Hi Johnson
I only tried the steps that Telson listed.
Maybe that's normal behavior with those steps?
It's such a small assembly, it was easy to just re-apply the constraints, and move on.
I can't publicly share the files.
Hi! Indeed, the steps Telson provided would lead to the behavior you are seeing. It is because Copy and Paste do not carry over the existing constraints. Only the component occurrences are pasted over. If you do Demote workflow, the constraints will survive.
Many thanks!
Hi! I guess you may have some constraint relationship among components. Try this. Go to Relationship folder -> suppress all constraints. Then demote. Does it work better now?
Many thanks!
If you have used this Assembly or have drawings you will cause:
That said this worked for me.