Can you create a cut feature in an assembly?

Russell_Lyons

It is quite common to create a welded assembly and then machine after welding.  A separate part or assembly is created for machining.  Is there a way to do this in OnShape?

alnis

You can't modify geometry within an assembly, but it sounds like you could do what you need in a Part Studio. Essentially, the division is Onshape is:

• Part studios define the geometry
• Assemblies define the motion

There are approaches that I can think of. For both, you'll want to first model the whole welded assembly within a single part studio with the Beams custom feature.

1. Create a configuration checkbox (or table if you want) to configure the suppression of all of the post-welding operations. This is simpler and keeps everything very neat, but if you have many post-welding operations, the configuration table/checkbox might get unwieldy and you do need to configure suppression for each feature separately. An advantage of this is that you have a single model/source of data to include in assemblies (e.g. with fasteners), so you can freely toggle the manufacturing operations with less concern about mates breaking, and exploded views will automatically "just work" between both configurations.
2. Derive all of the parts into a second part studio and do any edits there. When making the drawing, you can insert either/both part studios to show how everything goes together. With this method, you don't need to individually suppress any features, and you don't have to manually update a configuration table. However, it becomes a bit hairy when you start to add the parts to assemblies because there isn't any clean way to switch back and forth between pre/post-machining after welding.

Hope this helps! Let me know if you'd like me to put together an example.

Russell_Lyons

This is a work around that will work sometimes.  I think OnShape developers will want to add this to the list of improvements.  I have not used a cad system before that cannot do this as it is quite common to manufacture things in this way.  Consider a scenario where you have a steel forging that gets welded to a plate and then machined.  This same forging can get welded in many different assemblies and get machined differently to meet customer specs.

alnis

In that case, I would probably do it with derive features. Since the forged part will not be moving relative to the plate, it doesn't need the assembly environment to define its motion. In fact, I would probably model it as a multi-body part in Inventor or SolidWorks because it preserves the design intent as a single, final part (albeit it is manufactured by combining other parts). The welding is a step in the fabrication process of the single, solid part, rather than a motion-defining step, so that sort of change is more appropriate in a part environment in my opinion. Then again, I am a student who is still learning a lot, and I only have experience working on school-level projects, so I am probably making some mistakes in my reasoning!

Russell_Lyons

I'm thinking of a cylinder manufacturer.  They will have standard ends for their cylinders that will be welded to various rods and barrels and then machined after welding.  A cylinder manufacturer could easily use a forging in a 1000 different weldments.  I have no idea how you would handle that in OnShape.  In my case I have standard DOM tubes that I will weld into various weldments and then machine after welding.  The weldment essentially becomes a single part from a process standpoint and then gets machined afterwards.

lana

@Russell_Lyons
Please try In-context modeling https://cad.onshape.com/help/Content/in-context.htm
You can create a new part studio in context of the assembly, in part studio, make copies of welded parts, combine them in a composite part and make what-ever modeling changes are needed. Hope this works for you.

Prachi

Here's a work around for something simple like a shaft and welded end fitting by deriving 2 parts into a new part studio, You can boolean  them to one and machine material off and represent the weld.
Something like a welded table would be a lot of work. Better if we have a way to treat and assy as a weldment.
https://cad.onshape.com/documents/81cf8d5fab2f5bf37fdf9aa9/w/0c43eaa1e7778f35c1e38edb/e/d0d465135711076ba3aa5aad

matthew_stacy

@Russell_Lyons , I approached this problem by exporting the assembly and then importing that.  The import will create two document tabs, one of which is a Part Studio where you can model subsequent post-assembly machining steps.  You have the option to join these parts as a composite part (open or closed), boolean union them together, or leave them well enough alone depending on what best suits your purpose.

This is surely not a perfect work around.  Does it meet your current purpose?

• Example:  https://cad.onshape.com/documents/8e9b6ca98b6cabac6adf3f0d/w/63ce145b77540ceca0aba2c6/e/7c4e9f52383abfa127a8ab2a
  

mahir

alnis_smidchens said:

There are approaches that I can think of. 

1. Create a configuration checkbox (or table if you want) to configure the suppression of all of the post-welding operations. 
2. Derive all of the parts into a second part studio and do any edits there. 

Another option that's in between configurations and derived parts is making a copy of the part within the same part studio and applying your post weld features to the copy. Like a derived part, it's treated as a separate part. Like configurations, it's all in one part studio, but without haven't to remember which features to suppress. But you do have to be careful with your context (i.e. which body your features are applied to).

Prachi

Best option in the long haul is to have weldments as a feature for treating assemblies so that work arounds aren't necessary. Found this IR from 2017. I would use with some regularity.
Please cast your vote on this IR.
https://forum.onshape.com/discussion/6058/weldments-and-associated-tools