How do I hide weld features in drawing views?

[charlesKUCZ3]

I have searched for an answer, but can't seem to locate a suitable response.

The weld features that i placed in my model show in my drawings/shop details. The fabricator is not going to want to see all the weld features in the detail as it will only confuse them and lines will just run together. How can i make all of my welds in my drawing views invisible? Inventor Pro 2019

[blair]

I don't think you can. I tried a new View rep with the welds suppressed and they stay suppressed when you go back to another view. I did the same with Level of Detail and they stay in the suppressed state as well. 

I guess you could do a drawing with the welds suppress, then turn on the Defer Updates on the drawing sheet. It might work for you. I just hate having drawings that are in a Defer Updates state.

[mcgyvr · Accepted solution]

Simply edit the base view, go to the model state tab and check "assembly" 

[charlesKUCZ3]

Ha! Too easy. I would've never found that! Thank you.

[jtylerbc]

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@blair wrote:

I don't think you can. I tried a new View rep with the welds suppressed and they stay suppressed when you go back to another view. I did the same with Level of Detail and they stay in the suppressed state as well. 

I guess you could do a drawing with the welds suppress, then turn on the Defer Updates on the drawing sheet. It might work for you. I just hate having drawings that are in a Defer Updates state.

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@blair, you're thinking a bit too much of the welds as being like a part.  Welds are considered an assembly-level feature, so Suppressing acts the same as Suppressing an Extrusion in a part, rather than acting like Suppressing a part in an assembly.  View Rep doesn't matter, LOD doesn't matter, Suppressed is Suppressed when it comes to features.

However, if you right-click on the "Welds" line in the browser, you can turn Visibility off instead.  Then what you were trying to do with View Representations will actually work.  Additionally, you can right-click on this same "Welds" line, go to the iProperties, and use the "Weld Bead" tab to change the Appearance of the welds.  This doesn't really help with a drawing view, but I use it often to recolor welds to match the painted assembly.  This setting also respects View Reps, so you can have the welds look like welds in one, and be painted the same color as your finished weldment in another.

I use this method all the time when I need to get weld geometry out of the way for clarity, but still want to show post-weld machining.  @mcgyvr's suggestion about using the Assembly stage to show this will work in many cases, and is less work when it applies.  But it doesn't work out for situations when you need Machining features to remain visible, but Welds to be removed.

[blair]

Thanks, it didn't even look/think of the IDW environment this morning. Too much multi-tasking and not enough coffee.

🙂

[hncarle]

For our shop we NEVER put weld features into the model.  LOL our solution is "just say no."

[charlesKUCZ3]

You know, I thought about that. I am very new to inventor so i really don't know what i'm doing anyway, but i wondered what the point of putting welds in the model was anyway. I guess if I required very accurate weights or running simulations it may apply, but we are just fabricating some heavy duty machinery. Maybe it just wouldn't apply in some industries?

[jtylerbc]

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@charlesKUCZ3 wrote:

Maybe it just wouldn't apply in some industries?

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It can be even more selective than that.

At my company, we've had some issues in the past with interferences that weren't detected until fabrication, because someone didn't notice that a weld (which wasn't modeled) was going to be in the way.  For that reason, and some of us (including me) tend to prefer to model the welds.  It's much easier to catch an interference problem that you can actually see.

Additionally, I personally find that it's easier to keep track of what welds have been sized by modeling them, essentially using the model as the checklist for what welds haven't been decided on yet.  Similarly, having the welds shown graphically on the drawing makes it easier for me to keep track of what welds I have called out and which ones I still need to.  It also can come in handy for describing very specific situations, such as avoiding weld in a designated area.

However, not all of our users feel the need to do that, and we don't make it a requirement.  Even those of us who do tend to model the welds may skip it in some situations.  And even when we do model it, we may choose not to show it on the drawing if it creates more clutter than clarity.  Or we may omit showing the welds on the main views, but show them in detail views.

I would say that it is very situational, even within a single company, whether modeling the welds is actually worthwhile or not. 

[Sergio.Bertino]

Hello @charlesKUCZ3,

Thanks for your post.

Did the answer from @mcgyvr help you?

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

[Anonymous]

You can create a view representation and while being in that turn off the weld visibility by right-clicking on it. And while using the model in drawing, you can use that same view representation and it won't show welds in it. You can make a template file to keep that view representation with No weld for future use. I hope it helps.