How do you turn off visibility or suppress welds for use in drawing views

[jweiss1313]

I have an Inventor user who created a weldment.  He has three main pieces that he wants the fabricator to weld together first so he's created a design rep of the three parts and has created a drawing view that references this design rep.  He wants to only show the welds that apply to these three parts in this drawing view.  He is unable to turn the visibility off on individual welds.  He can suppress individual welds.  He cannot get the LOD to work with the suppressed welds.  He created a LOD and suppress all but two welds.  When he selects the master LOD on two welds show up.

Can anyone help us to create this drawing view so that on three parts of a larger weldment are visible and only the weld that apply to these three parts show up in the drawing view.

Thanks to whoever can help us.

John Weiss

CAD Admininstrator

Follett Corporation

[Anonymous · Accepted solution]

Demote parts 1 and 2 to a subassembly and then place the first series of welds in this subassembly. Place the second series of welds at the top level assembly between part 3 and the subassembly.

Then in the drawing view of the top level assembly, edit the view and go to the Model State tab. Set the Weldment  option to 'Assembly', this will show the top level assembly as it existed before the second series of weld was created.

[Anonymous]

I think I confused the issue with the numbered parts, but basically just place all of the components to be welded first into a subassembly, then in the drawing view of the top level assembly, edit the view and go to the Model State tab. Set the Weldment  option to 'Assembly', this will show the top level assembly with all parts, but only the welds in the subassembly.

[Anonymous]

BMiller,

quick question. Where did you download this file? I see not attachment in the original post.

Dennis

[Anonymous]

Hi Dennis,

There was no file, I was speaking to the description the OP made of the weldment.

[jweiss1313]

Dennis,

Here is the dataset for this issue.  You will see on sheet 2 of the idw that the user is trying to show a sub-assy without creating an actual sub-assy (.iam).  He's trying to have one assembly file and be able to show a two step welding process that include welding two parts on the shaft ends and then showing the remainder of the the assy welded.

I'm attaching the idw to this post and the assy and parts to a second post.

John Weiss

CAD Administrator

Follett Corp

[jweiss1313]

Here are the components and the weldment assy.

[Anonymous]

John, always indicate what version of Inventor is being used...

[jweiss1313]

Sorry - we are using Inventor Pro 2010

[Anonymous]

1. Activate Master Level of Detail

2. Create New Level of Detail

3. Save

4. With new level of detail active, suppress the desired welds.

5. Save

6. Copy the LOD to a View Rep

7. Save

In the IDW, apply the new View Rep to the view. (Edit View).

[Anonymous]

It helps to put that in your signature for future use.

[Anonymous]

I'd like to change my previous answer from what I said (use a subassembly), to what Dennis said (use a view rep)! 🙂

Actually both would work, but Dennis' solution is the better choice.

[jweiss1313]

Hi Dennis,

I followed your instructions and created the LOD and design rep and all the parts suppress and un-suppress properly.  When I suppress the welds in my new LOD they stay suppress is all LOD's including the master.  The welds do not reactive to different LOD's like the components do.

Please try your process on my dataset and let me know if you see the same thing as I do.  I want to see all welds in all views except the sub-assy view in the middle of sheet 2.

John Weiss

CAD Admin

Follett Corp

Inventor Pro 2010

[Anonymous]

I did it without issue in 2011, however, it should work the same way in 2010. See attachment.

I'll be out of the office for most of the day, but if you cannot get it to work, let me know and I'll redo in Inventor 2010 or contact you.

[jweiss1313]

Hi Dennis,

I just tried again and the welds are not being controlled by the LOD.  I've followed you instructions twice and either the welds are suppressed in all LOD's or they are on.  It doesn't seem like LOD can control the weld suppression in Invento 2010. 

If you can try this in INV2010 I would really appreciate it.  I'm pretty good at Inventor and this does not seem to work.

John Weiss

CAD Administrator

Follett Corp

Inventor Pro 2010

[Anonymous]

Hi guys,

Okay I'm gonna waffle on this again (maybe I'll go into politics soon!).

I looks like when I ran through Dennis' steps this morning, I didn't update the drawing views and therefore didn't catch that the weld reapeared in the view when unsuppressed.But I just ran though it again and sure enough it's an all or nothing thing.

So, I'm back to my earlier recomendation of using a subassembly for the 3 parts (00958421, 00102137, 00958413) for the first step. If the concern is that the subassembly will list in the BOM, just be sure to set the subassembly as Phantom. Weld beads 1 and 14 will need to be removed from the top level assembly and placed in the sub.

And then the view on sheet 2 needs to be set to 'Assembly' in the Model State area, this will show the top level assembly as it existed before the second series of welds were created.

I did this all in Inventor 2010

Okay, that's my stand on this for now (until Dennis comes back and shows us a better way!)

I'm Bmiller63 and I approve this message.

[jweiss1313]

I have to agree with you.  I've tried your workflow and everthing worked great.  I was hoping that I would be able to do it without having to create a sub-assembly and use LOD like Dennis suggested.  I would be really curious to see if this is an improvement to INV2011.

Thanks for all your help!

John Weiss

[Anonymous]

It worked in 2011. You can see selected welds in the attachment. I'll try it again in 2010 when I get a chance.  Tell me which welds (by name) you want to preserve.

[Anonymous]

Just redid th eexercise in Inventor 2010 SP3. Same result. I can supress/unsupress welds at will.  Here's the 2010 result.

Sheet 2 View 16.

[Anonymous]

but can you show welds 1 and 14 only on sheet 2 and then show all of the welds on sheet 3?

Sheet2 being weld stage 1 and sheet3 being weld stage 2.

It seems that you can either have welds suppressed or not have them suppresed there is no way to represent the same weldment in two different views at two different stages. The view rep does not hold the weld supression state when toggled back on/off.