Community
Inventor Forum
Welcome to Autodesk’s Inventor Forums. Share your knowledge, ask questions, and explore popular Inventor topics.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

how to convert the weldment assembly back to regular assembly template

26 REPLIES 26
SOLVED
Reply
Message 1 of 27
linuskotte
20621 Views, 26 Replies

how to convert the weldment assembly back to regular assembly template

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

 

26 REPLIES 26
Message 2 of 27

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


Message 3 of 27

I found that I can just copy parts from weldment to new assembly. By copying all relations are converted too.

Message 4 of 27
shawn.payne
in reply to: aaniaa13

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.

Message 5 of 27

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?

Message 6 of 27

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!

 



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Message 7 of 27

That doesn't work as the whole point is to remove the weldment completely
Message 8 of 27
cdraghi3
in reply to: linuskotte

The actual solution is a combination of demoting and copy/paste feature. This is for Autodesk Inventor 2015.

  1. Open the weldment.
  2. Left click on the background and drag your cursor across the entire weldment assembly.
    • This should highlight all the parts in the actual display. 
  3. 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.
  4. You will notice that inside your weldment, you now only have one item: an assembly of all the items that were just demoted.
  5. Now you need to right click on this assembly in the BROWSER and select COPY.
  6. OPEN a regular assembly file.
  7. Right-click and PASTE the assembly into the new assembly file. 
  8. Now EXPAND this assembly. 
  9. 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.
  10. You can now select the original assembly item that was copied from the weldment and DELETE it. 
  11. Save this assembly!! 
  12. You are done! 
Message 9 of 27
cdraghi3
in reply to: stephenjohns00

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.

  1. Open the weldment.
  2. Left click on the background and drag your cursor across the entire weldment assembly.
    • This should highlight all the parts in the actual display. 
  3. 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.
  4. You will notice that inside your weldment, you now only have one item: an assembly of all the items that were just demoted.
  5. Now you need to right click on this assembly in the BROWSER and select COPY.
  6. OPEN a regular assembly file.
  7. Right-click and PASTE the assembly into the new assembly file. 
  8. Now EXPAND this assembly. 
  9. 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.
  10. You can now select the original assembly item that was copied from the weldment and DELETE it. 
  11. Save this assembly!! 
  12. You are done! 
Message 10 of 27
stephenjohns00
in reply to: cdraghi3


@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.

  1. Open the weldment.
  2. Left click on the background and drag your cursor across the entire weldment assembly.
    • This should highlight all the parts in the actual display. 
  3. 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.
  4. You will notice that inside your weldment, you now only have one item: an assembly of all the items that were just demoted.
  5. Now you need to right click on this assembly in the BROWSER and select COPY.
  6. OPEN a regular assembly file.
  7. Right-click and PASTE the assembly into the new assembly file. 
  8. Now EXPAND this assembly. 
  9. 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.
  10. You can now select the original assembly item that was copied from the weldment and DELETE it. 
  11. Save this assembly!! 
  12. You are done! 

This still loses all mates to the origin planes/axes.

Message 11 of 27

Hi! Are you using Inventor 2015 or earlier? If you are on newer releases, demoting components will preserve constraints between demote participants.

Many thanks!



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Message 12 of 27

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.

Message 13 of 27

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

Message 14 of 27
fatherof3
in reply to: Telson.Hadden

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.

 

Message 15 of 27
johnsonshiue
in reply to: fatherof3

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!



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Message 16 of 27
fatherof3
in reply to: johnsonshiue

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.

 

Message 17 of 27
johnsonshiue
in reply to: fatherof3

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!

 



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Message 18 of 27

it will not demote the component pattern.

Message 19 of 27

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!



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Message 20 of 27
drawings
in reply to: linuskotte

If you have used this Assembly or have drawings you will cause:

  • Lose any weldment specific features.
  • Unresolved Files since it doesn’t recognize the file. You will have resolve them for the new assembly to be accepted.
  • Constraint issues in these assemblies.
  • BOM rearranged and renumbered.

That said this worked for me.

  1. Create a new assembly in the ‘weldment assembly’
    1. Make it a normal assembly
    2. Ground and root the new assembly
    3. If you are using Vault, check out the ‘weldment assembly’ before you over write it or Inventor will through up a road block.
  2. Move over mates to the new assembly.
    1. Have "Display component names after relationship names" checked in the Assembly tab of Application Options.
    2. Expand both the top assembly and the new assembly origins to expose all elements and their mates. Move all of the origin mates over one at a time from the browser assembly planes.
    3. Edit each Mate and be sure you select the correct half of the mate. They are in the order displayed after the relationship name.
    4. Using that selection choose the corresponding plane or axis in the new assembly. Don't change alignment or disconnect the other selection or you will lose your mate and may find your model rearranged. Undo if you do.
  3.  Move Components into the new assembly.
    1. If moved first all the mates would refer to the new assembly instead of the components and will not be able to move the origin mates to the new assembly.
    2. All Patterns that use the origin features for an reference will have to be edited to the new assembly reference.
  4. Replace old assembly with new
    1. Save new assembly as a new name, choose old Assembly name and add a – after it.
    2. Close old assembly without saving, include all files that reference it.
    3. Open old assembly as it was and compare the two.
    4. Make any further changes to the new assembly.
    5. Close or Save old assembly under a new name as a backup.
    6. Save New Assembly under the old assembly’s name and check in if using Vault.
  5. Open and fix any issues if already used as mentioned at the first.
    1. If it is used in one assembly it may work to do a side step procedure instead.
    2. Open the upper assembly.
    3. Create the new assembly in the upper assembly.
    4. Move the mates from old to new assembly origins
    5. Move components, etc.

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report