level of detail

[SolidCreative]

Is it possible to suppress features of a part in a drawing? For example. I made two drawings of a weldment, one for the welder, and one for the machinist. I didn’t want to show holes or machined feature to the welder. Could I suppress those features in the part using level of detail or configurations?

Flame cut drawings would be just simple plates, and not pieces of Swiss cheese... Umm.. I love my cheese!

Thanks

Matthew

 

[dzine]

Matthew,

I think you are seeing two issues here.
One is the different configurations of the assembly, and one is the configuration of parts.

Assembly: You need to do this in two distinct steps.
Step one would be the weldment of 2 or more parts, and subsequent drawing detail (no holes, no machining).
Step two would be to create a derived part of the weldment, and do the holes and machining on the new ‘part’ (which is actually a weldment). You can then create a drawing of the new part, with the machining detail.

Part only: In my experience, you are best to do this in two steps also (for flame cut, then machined parts).
Step one- Create the part with the profiled hole (which is smaller than the machined hole will be), but do not create any drilled holes. Then create a ‘Profile’ drawing, from which you can export the dxf easily etc.
Step two- Make a new derived part from the ‘profile’ part and do all the machining and hole features. You will be able to have another drawing now, with the machined details.

With solid modelling, you are generally best to design the part exactly how they would do it in manufacture. Both the process above simulate that. i.e. when the welder completes his (or her!) task, the assembly essentially becomes one part for the machining process.

I hope this helps, but I am sure others will have differing opinions

Hayden

 

[SolidCreative]

Thanks for the detailed response. I was hoping to stay away from derived parts though, as they require an additional filename.ipt

I've just attempted to create an iPart for each member of the weldment that will need to be shown in progressive states. It seems to work pretty good, as I can flip between iParts inorder to show before and after machining

Matthew

 

[brengine]

If you do it as a Weldment Assembly like the Help suggests, there is a Representations branch at the top of your Feature Tree that separates the Welded state from the Machined state.

I am new to Inventor, so I really can't say which method I prefer.

Ken

 

[rollupswx]

Do it exactly as done on real parts. If machined feature occurs before welding it must be in ipt.
If machined feature is done at time of welding (Preparations) do it in weldment iam. Then weld, then post-welding machining in weldment iam. When making an idw drawing from the weldment iam you will be prompted for the stage of manufacture to show in the view.

 

[SolidCreative]

I never really knew the advantages of weldment assembly’s, but yeah, that’s the best option for what I’m trying to accomplish