Best Practice for Welded Assembly 1

[matthewcsmith]

I am working on creating an assembly of parts which is machined. What I'm looking for is others experiences to try to determine a best practice for this type of a part. The finished part is created by machining two parts, welding them together, and then finish machining additional features.

I would like to be able to completely specify the two parts which will be welded so I may provide machining drawings/details independent of the finished machine drawing of the assembly.

As a note, I am using SW 2014 with EPDM for file management.

Matt Smith
Mechanical Engineer

 

[Jboggs]

Are you familiar with configurations (as-machined vs as-welded) and relative views of individual bodies? Those tools would allow you to keep all the information in a single part file (not an assembly file) and still be able to show the various stages of fabrication for individual pieces.

Create your weldment part using non-merged bodies as usual. Create configurations showing initial machining, as-welded, and final machining.

In the drawing, the first thing I would do would be to place views showing the as-welded configuration so I can finalize the weldment cut-list. Then I would create relative views of the individual pre-machined bodies, probably on separate sheet(s). Then create another sheet to show the finished machined part with all the final machining dimensions and GDT.

If you don't yet know how to do any of these steps there is a process to go through. More than I wanted to jump into here but I can help if you need it.

 

[ctopher]

If you don't know how to do weldment's, you can do Jboggs suggestion with config's.
Each part has the machining features in one config, and the after weld machining in another config.
Make an assy, and it's dwg, calling out the welding.

Chris, CSWA
SolidWorks 14
SolidWorks Legion

 

[matthewcsmith]

Thank you for the suggestions. I have previously used configurations for this type of component. I have several different versions of this part which use the base welded assembly as the starting part. Then through additional welding and/or machining operations it is made into other finished parts. Typically I would have treated them as an assembly with multiple instances of the same part with different configurations initialized for each instance.

Would you treat the as welded part as a part or an assembly? I am not familiar with bodies, but it feels like these could be used maybe? Can unmerged bodies be used somehow to keep the as-welded as a part, but still show the joints? I want to be able to clearly show all the steps/drawings/parts.

I am also familiar with inserting a part into a part (typically done with a casting to be machined into a finished part). Unfortunately, this is not available with an assembly.





Matt Smith
Mechanical Engineer

 

[TheTick]

Given the amount of post-assembly machining involved, I would consider assembling this within a part file using Insert --> Part. This way, you have full access to all the cutting options that may not be present in an assembly file.

You sacrifice a little by not having a cut list or BOM built in (at least it's only 2 parts, easy to do manually), but you gain access to all SW Part features.

 

[ctopher]

I would make it an assy to keep the references of the machined parts.

Chris, CSWA
SolidWorks 14
SolidWorks Legion

 

[matthewcsmith]

TheTick - I had never inserted more than one part into a part. Thank you for the suggestion.

ctopher - Once it is an assembly there are some cutting options (wrap in this instance) which I would like to use that are no longer available.

Matt Smith
Mechanical Engineer

 

[TheTick]

I've done this a few times on wood furniture that was routed after assembly.

 

[matthewcsmith]

As a sidebar to the discussion here, why would you use a multibody part?

Matt Smith
Mechanical Engineer

 

[Jboggs]

If you aren't familiar with multibody (un-merged) parts, I would strongly encourage you to learn more about them. You have to learn the particulars about how it affects patterning, mirroring, extruded cuts, etc. but it is an extremely useful approach for my work. In fact, its my default setting now. It creates a lot more options of "how to do stuff" for me. One reason is that it more closely tracks with how things are done in the real world.

For example, say in the real world you drill a hole thru one piece and then weld it to another one so that one end of the hole is covered. You have created a blind flat bottom hole. In SW you create the part using two Extrude Boss commands. If those two Extrude Bosses are "merged", they are one body. A Hole Wizard drilled hole includes the conical point at the bottom, just as a normal hole does in the real world. There is no easy way to drill through one welded part without leaving that conical point cut in the mating part. But Hole Wizard (as most other cut features) allows you to select which bodies the feature applies to. If you modeled those two Extrude Bosses as unmerged bodies, you can insert a Hole Wizard hole all the way thru one body and have zero effect on any other body.

A section view of merged bodies shows no separation line, because there isn't one. A section view of unmerged bodies will show the edge between them.

In drawings, one of the options in the Relative View command is to select which body or bodies to show in that view. That way you can show all the cutting and fab details to be done on any single piece before welding. It is our default method of showing weldment detail pieces.

When you declare a part to be a weldment, SW does several things. It sets all future extrusions to non-merged unless you select otherwise. It converts the Bodies List to a "Cut List". It also creates default configurations "as welded" and "as machined".

We use it a lot!