Weld Symbols - not parametrically linked to model?

[Hoz]

Hi All,

So maybe my memory is failing.... but it turns out if you:
- add weld beads to in your 3D model (Insert > Assembly Feature > Weld Bead)
- import them to your 2D drawing views (Insert > Model Items)
- change the weld properties in the 3D...

The weld notes don't update in the drawing....so they're not parametrically linked. Where this bites is if you're using the notes to specify weld length for example, then make a change to the 3D model, the 2D weld length text remains the same....

I'm playing around with adding a dim, then creating a note referencing the dim and grouping that dim to the weld note.... pretty messy. Anyone out there got any better workarounds?

Cheers,

[mattpeneguy]

Hi All,

So maybe my memory is failing.... but it turns out if you:
- add weld beads to in your 3D model (Insert > Assembly Feature > Weld Bead)
- import them to your 2D drawing views (Insert > Model Items)
- change the weld properties in the 3D...

The weld notes don't update in the drawing....so they're not parametrically linked. Where this bites is if you're using the notes to specify weld length for example, then make a change to the 3D model, the 2D weld length text remains the same....

I'm playing around with adding a dim, then creating a note referencing the dim and grouping that dim to the weld note.... pretty messy. Anyone out there got any better workarounds?

Cheers,

Years ago I got the impression that welds were like Toolbox gears. Good for "representation" and not much else. Since then I've always manually added weld symbols to my drawings. Maybe someone else here can give you a good workflow, but when I looked into it (maybe about 8 years ago) I didn't find one that seemed worth it.

[Frederick_Law]

3D weld is hit or miss. I think some use it for weld weight calculation. Most of the time I can't get the weld I need.

[mattpeneguy]

3D weld is hit or miss. I think some use it for weld weight calculation. Most of the time I can't get the weld I need.

For that kind of thing, what about just adding fillets manually? I guess it depends on the complexity of the weld and part, but when you don't have a good tool, you have to do what ya gotta do...

[Frederick_Law]

I'll have fillet or other weld prep (J, V etc) for machining.
I've seen model from other software will all the weld beads.
A real pain importing.

[Hoz]

Thanks for the replies; yeah I was referring to just the annotations in the 3D:

I abandoned the older 'Fillet Beads' ages ago; loads of extra bodies, all called Part1, Part2 etc... which is a real pain when it comes to file management.... that combined with the body errors that often occur....

My VAR tells me there's an open ER to link Weld Beads (the annotation type) to the drawing so they'd update parametrically like normal dimensions do, so watch this space. For now it's back to doing it all manually in the 2D I think.

Cheers

[Glenn Schroeder]

I also don't add weld beads in my models. All they're good for is to clutter up drawings and make them more difficult to decipher. I just add weld symbols in the drawing.

Also, I got discouraged once when I did add them because a client asked me to put the total weld bead length on the Drawing. No problem, I thought. Wrong. The information is there in the model, but there's no parametric way to get it into the Drawing (or at least there wasn't then; it was probably 10 years ago).

[Hoz]

a client asked me to put the total weld bead length on the Drawing. No problem, I thought. Wrong. The information is there in the model, but there's no parametric way to get it into the Drawing (or at least there wasn't then; it was probably 10 years ago).

I had the same issue, so here's my workaround

For simple, linear weld lengths:
- Create a layer called 'hidden' or something
- Add a normal linear dimension to where the weld line is
- move this dimension to the 'hidden' layer
- insert an annotation without a leader, then click on the newly created dimension to call it up in the annotation
- insert your weld note, with a few spaces in your weld length box
- position the annotation correctly WRT the weld note and R-click > Group them together
- hide your hidden layer

Voila. Horribly convoluted but it works and should update if your 3D changes.

For more complex weld lines, I've had to sketch a string of entities in the 2D view, make them a Path, then add > Path Dimension to read the length. This can be grouped in the same was as for linear dimensions above....except there's a bug in 2022 (sp1) at least where path dimensions don't hide with hidden layers, so you have to R-click > Hide the dimensions manually.

Crap, but it does work. Breathe out....

[JSculley]

Hi All,

So maybe my memory is failing.... but it turns out if you:
- add weld beads to in your 3D model (Insert > Assembly Feature > Weld Bead)
- import them to your 2D drawing views (Insert > Model Items)
- change the weld properties in the 3D...

The weld notes don't update in the drawing....

What do you mean by 'weld note'? Do you mean the weld symbol? If so, I'm not seeing the behavior you describe. If I add a weld bead to an assembly, insert model items in the drawing and then go back and edit the weld bead (e.g. change the fillet size), the weld symbol in the drawing updates as expected (SW 2022 SP2).

Here's my model:

Here's the drawing:

Change the model:

The drawing updates:

[JSculley]

I also don't add weld beads in my models. All they're good for is to clutter up drawings and make them more difficult to decipher. I just add weld symbols in the drawing.

Weld beads as an assembly feature don't clutter up drawings at all. They don't even show up unless you use shaded views in the drawing.

Also, I got discouraged once when I did add them because a client asked me to put the total weld bead length on the Drawing. No problem, I thought. Wrong. The information is there in the model, but there's no parametric way to get it into the Drawing (or at least there wasn't then; it was probably 10 years ago).

Weld tables have been around since SW 2012 and they show you the total bead length:

[Hoz]

Thanks for the replies.

JSculley - I'm talking about using Insert > Assembly Feature > Weld Bead because this links the length of the 3D joint to the weld symbol:

When I then import the weld symbols produced into the drawing (Insert > Model Items ) it pulls the weld path length through but doesn't update when the 3D model is modified.

I guess this is different to what you're doing?

[JSculley]

Here's a weld:

and the drawing:

Change the model:

and the drawing updates:

If this isn't working for you, something is wrong. Out of curiosity, if you insert a weld table, do it not update either?

Also, can you upload a sample assembly (with parts) and drawing? I would like to see if it misbehaves when I work with it.

[Hoz]

Thanks for the reply and screengrabs. I've just tested it on a new file and it works just like your explanation.....so guess there's something wrong with the real asm file I'm working on as I follow the same workflow and even though the annotations in the 3D update correctly, the imported model items don't update in the 2D.... Unfortunately I can't upload the files due to IP stuff, but thanks for the offer - hopefully this is just a one off corruption or something...

Something else related, (when it's working properly) the weld lengths do update if I manually update the weld bead properties in the annotations folders, but they don't seem to permanently linked to the 3D geometry as if I change the component dimensions (part below was 120mm, increased to 150mm) the weld bead length stays 'fixed' to the original geometry, even though the 'Weld Path' selection edge updates to the new dimension.... is this just me?

Weld table does seem to match the annotations though:

Which is one relief. Cheers

[JSculley]

Thanks for the reply and screengrabs. I've just tested it on a new file and it works just like your explanation.....so guess there's something wrong with the real asm file I'm working on as I follow the same workflow and even though the annotations in the 3D update correctly, the imported model items don't update in the 2D.... Unfortunately I can't upload the files due to IP stuff, but thanks for the offer - hopefully this is just a one off corruption or something...

Depending on the age of the file, it could be a Crusty Old Template problem. If you have any anchors in your sheet format, you can right click on them and select 'Properties' to see the date when the template was made:

Something else related, (when it's working properly) the weld lengths do update if I manually update the weld bead properties in the annotations folders, but they don't seem to permanently linked to the 3D geometry as if I change the component dimensions (part below was 120mm, increased to 150mm) the weld bead length stays 'fixed' to the original geometry, even though the 'Weld Path' selection edge updates to the new dimension.... is this just me?
image.png

When you select 'From/To' you are explicitly telling SW where the weld starts and stops. If you want the weld to encompass the entire edge, just uncheck the From/To checkbox. The weld length will disappear from the symbol, but that is because the weld is assumed to be along the entire edge when no length is specified. Showing the length on such a weld would be redundant.

If you want your weld to change parametrically, but you don't want it to encompass the entire edge, you can create a sketch and use that for the weld path. But your symbols won't show the length. There is an enhancement request that would fill this gap in functionality:

SPR 752806: Weld bead 'From To' definition should have an option to use a vertex instead of a numerical value or a second distance option instead of bead length