View Rep and weldments

[karthur1]

I would like to be able to turn the visibility of the welds off and control it with a view rep. How can I do that?

When working in a weldment, I would like to demote some of the parts to a sub-weldment. When I do this, the parts are demoted to a "standard" assembly and I loose all my welds between the plates. Is there a way to demote parts in a weldment and have them demoted to a weldment with the welds?

[Anonymous]

Give this a try. Create a new View Rep then right click on the "Beads"
folder and uncheck the "Visibility" entry. This will get saved in the view
rep. Unfortunately it's an all or nothing deal because it doesn't look like
you can individually toggle visibility for each weld.

As far as demoting goes you can select a weldment template to demote into
but you are going to lose your weldments regardless of what you do. Just as
in the assembly environment you cannot demote components and retain the
"assembly level" features on that component weldments fall into the same
paradigm.

Thanks.
--
Gary Tafoya
Inventor Assembly QA


wrote in message news:5882763@discussion.autodesk.com...
I would like to be able to turn the visibility of the welds off and control
it with a view rep. How can I do that?

When working in a weldment, I would like to demote some of the parts to a
sub-weldment. When I do this, the parts are demoted to a "standard"
assembly and I loose all my welds between the plates. Is there a way to
demote parts in a weldment and have them demoted to a weldment with the
welds?

[signmeup]

4 years later and it's still all or nothing with weld visibility

[mtungseth]

It is now an additional 3 years later and still all or nothing with weld visibility.

Or am I missing something?

My issue is this: one weldment assembly, want 2 drawings showing different parts of assembly. 

I can control which parts to have visible using view reps, but all welds will be visible, destroying the view on the drawing.

Workarounds anyone?

Marius

[blair]

You can Suppress individual welds and parts within the LOD and then create your drawing views using the desired LOD. Normally LOD's are a memory tool to reduce the system load but it seems to work for this.

[signmeup]

You cannot suppress welds within an assembly under an LoD. I think that is
what has been requested.



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[blair]

Just expand the Welds folder, RMB select the required weld and Suppress. It worked for me last night before I posted the solution. I'm on IV2016 so I don't know it that functionality is in older versions.

[jtylerbc]

I haven't tried it in 2016, but it doesn't seem to work that way in 2015.  LOD's and suppressed welds are independant.  If you suppress a weld, it's suppressed everywhere no matter what LOD you switch to.  Same is true for features created in the weld Machining level.

[blair]

Something like this: http://autode.sk/1KGrbaU

Then create your drawing views using the LOD's you require.

[jtylerbc]

blair,

Your video stops before where the problem exists (in 2015 and older, at least).  What happens to the welds when you switch back to Master LOD?  In 2015, when you suppress the welds, they are suppressed in all LOD's, not just the active one.  If you then unsuppress them in the Master, you're simultaneously turning them back on in the "welds removed" LOD.

Is that behavior different in 2016?

[blair]

Same as IV2015, you need to manually un-suppress the welds.

[jtylerbc]

So then what is the LOD doing for you (with regards to the welds)?  When you unsuppress the welds manually in Master, it messes up your new LOD also, so the new LOD might as well not exist (again, with regards to the welds - I realize your example also suppressed parts).

The weld suppression isn't saving with the LOD's.  All LOD's show the same weld suppression settings.  So you can't make a drawing view that has the suppressed welds omitted, and another view where they are shown.  All views will show the same welds no matter what LOD they reference.

If I'm missing something here and there is a way to make this work, please correct me.  I've tried figuring out a way to selectively show welds many times and have always come up empty.

[blair]

Correct, I guess, you could create the view with the LOD, then select the "Differ Updates" for the view in the drawing to lock the drawing view with the suppressed parts and welds.

I guess "Weldments" due to their "inseparable" nature within Inventor just don't behavior nicely. Since I'm not a big fan of the "Differ Updates" I wouldn't want to use this setting as other aspects of the model could become frozen on the drawing as well.

[jtylerbc]

Yeah, I wouldn't want to do it that way either.

I don't think this is technically an issue with weldments at all.  All assembly-level features act this way (not interacting at all with View Reps or LOD), even if they are not made in a weldment assembly.

It seems it is a limitation with assembly features in general.  Welds behave this way, but so do weldment Machining features, as well as extruded cuts in a regular assembly.

[signmeup]

I think the answer is to set the view in the Inventor drawing to not show
any welds and then add welds using weld symbols.

That solves the drawing problem but leaves modelling in a mess still with
welds hovering in mid-air.



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[signmeup]

I think the answer is to set the view in the Inventor drawing to not show
any welds and then add welds using weld symbols.

That solves the drawing problem but leaves modelling in a mess still with
welds hovering in mid-air.



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[mtungseth]

---

@signmeup wrote:
"I think the answer is to set the view in the Inventor drawing to not show
any welds and then add welds using weld symbols."

The answer might well be to not use the weldment features at all if you don't have to.

I remember the introduction of weldments in Inv 6 I think it was. I gave it a try at that time, but abondoned it quickly because of all bugs and lack of control.

Today I recognise many of the same problems still appear, i.e. visibility of weld symbols in the model view.