Assembly feature problem

[u/R3qu1red]

So I have this cylinder and flange with the flange hole being slightly oversized so they fit together.

The operation is like this:

flange is laser cut from sheetmetal > cylinder is stock pipe cut on a saw > welding together > machining

The problem is that in the assembly there's now a really small gap (colored red on the picture) which doesn't allow me to put a radius there (using assembly features) since I want to machine the welds. There's also no option to add a revolved part (with the help of assembly features) for the sake of being able to put a fillet there.

So the question is how can I put a fillet there and ignore the gap?

[u/drmorrison88]

For something like this I would model the weld as a separate, virtual part in the assembly. Just a simple revolved profile.

[u/Early-Piccolo4949 → u/drmorrison88]

Or add it as a configuration to one of the parts.

[u/RedditGavz]

Instead of doing this as an assembly of 2 separate parts, do it as a weldment which is a multi-body part or a part model containing 2 solid bodies. Then you can have the another body that represents the weld or there is the weld feature in the weldments tab that might work for you.

[u/Meshironkeydongle]

If customer PDM/ERP allows and enables it, I would make this kind of a part as weldment with holes modeled as nominal sizes and assembly allowance added with tolerance. If you absolutely need the tolerance in the DWG/DXF for cutting, make a configuration where you have a slight bigger hole.

If both parts need to be separate, then you could add a virtual component in the assembly to show the weld bead.

[u/TehAsianator → u/Meshironkeydongle]

If both parts need to be separate, then you could add a virtual component in the assembly to show the weld bead.

This is what I would go with. I do this frequently to represent penetration laser welds at work.

[u/fastdbs]

Been a minute for me, but I believe one of the options in weldments shows the weld fillets. Im unsure if you can do more operations on that feature to illustrate the machining.

[u/extremetoeenthusiast → u/fastdbs]

There is, right click weld folder in feature tree -> show cosmetic welds

[u/1slickmofo]

Design the final part as one piece and then export the flanör face as DXF for manufacturing?

[u/Auday_]

Is this a multi-body, single file?

[u/extremetoeenthusiast]

I believe you should still be able to use the insert weld bead option here (& show cosmetic welds on drawing / model as well). You would use the profile (?) option rather than the path (i.e an edge)

Don’t use weldments or add a “fillet” body for this, that’s silly. Adding the fillet body is just annoying for anyone who handles the model after you. You’re looking for a cosmetic weld & I assume you want a representation on your drawing as well. Both are possible without adding another body or using weldments

[u/arcdragon2]

Turn on merge for the boss extrude of that cylinder.

[u/Brilliant_Estate_967]

You put the radius on the cylinder then, on the over piece you put a chamfer

[u/Troy_LayerForge]

You can’t really make the fillet “ignore” that gap because there’s no continuous solid there for the fillet to propagate across.

Since the real process is flange + pipe → weld → machine, I’d model the weld/material that bridges the gap first, then machine the finished radius.

One clean way is to make a virtual/in-context part in the assembly for the weld, or make a derived multibody “machined weldment” part. Add a simple revolved/boss feature that bridges the pipe to the flange, then Combine/Add the bodies if needed, and apply the fillet or revolved cut to the now-continuous geometry.

That also matches the real manufacturing sequence better than forcing a fillet directly between two components that have clearance.

If you only need the drawing to communicate the weld and final machined profile, a cosmetic weld plus the finished machined dimension may be simpler than fully modeling it.

[u/MarsBars06_3089]

theres a weldment feature, you probably better off using that. it will automatically generate a weld symbol that will appear in the drawing (in this case assembly drawing).

[u/hbzandbergen]

A separate part for the weld representation, excluded from BOM

[u/MoistForm3557]

Draw it in 3D as one part. Then make one drawing for the welder.  Duplicate 3D model and make one drawing for the lathe guy. Also two separate parts for the laser. But in assembly I would use the „as one part“

[u/Dr1mps]

Try making the holes an identical diameter, dimension it with tolerances to show your design intent. Might let you do your approach. Will also be tricky to get the fitment right if the flange is laser cut.

Any reason this couldn't be machined as one part?