Drawing - Section - Reference parts?

[mthomas]

In a drawing Is there anyway to section (and show the hatch pattern) on reference components?

[VinodBalasubramanian]

Hi,

Is this what you are looking for,

http://www.cadalyst.com/cad/inventor/add-reference-components-your-assemblies-10231

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[mthomas]

Not really. I understand how to create reference parts and that is working fine. It's when I create a drawing view of an assembly that contains reference parts, then section that drawing view. I am using the option for my reference parts to be displayed as parts and it sections the reference parts, it just doesn't show the hatch pattern on the reference parts

[VinodBalasubramanian]

Thanks for the update. Can you provide me a sample model and drawing. Also provide me steps on what you have done with the drawing. This would help me to understand the issue better.

[SteveMDennis · Accepted solution]

Vinod,

 I think I understand what Mike is saying.  Have a simple assembly that has 3 parts all in the relatively same plane, make the outside ones reference (under iProperties in the assembly context).

Create a base view of that assembly (adjusting the view margin so that you can see the outside reference parts.

Even if you say "As Parts" under line style in the view dialog, we don't crosshatch the reference parts.

Right Mike?

If I have it right Mike, there is no way to accomplish what you are asking for.  The As Parts option is simply which layer do you want the reference geometry to appear on basically.

Reference parts still have several baked in rules that are not overridable, such as not contributing to mass properties, not being sectioned, etc.

[harco]

You might try a derived phantom part, this should keep goemetric updates from original part but keep it out of the BOM.

You should be able to section, yes it's a work around but if it gets what you want.

Other than that sketch and fill.

[mthomas]

Thank you for the response and the suggestion. A phantom part might work in this situation, it is definitely worth investigating

Mike

[SteveMDennis]

Mike,

Help me understand your workflow a bit more please.  Our original intent was that reference parts were likely from  a vendor or other source and likely would be imported bodies probably without design intent like a shrinkwrap, etc.

We were thinking that there is no need to crosshatch such parts because the internals would likely not be correct anyway and this way you know they are not part of your design.

Any insight into your intent or workflow would be nice.

Thanks

[mthomas]

In the drawing that prompted this question it was a modification of an existing design that the customer already had. What we were attempting to show were the new parts that were added to the weldment and where they needed to be welded. As we don't want to show the existing parts in the BOM we tagged them as reference. However having the existing parts (reference) not section made the views difficult to understand, hence wanting to see the cross-hatching.

Hope this makes sense

Mike

[SteveMDennis]

That makes perfect sense Mike. Not a workflow we had ever thought of.

I wonder if a property of "Not in BOM" and/or "Not in Mass Props" would be valuable? Then you could set them independently from reference...

Reference has the nasty side effect of the whole Margin value. (Don't get me started on that!)

Thanks,

[mthomas]

Personally I think reference works exactly how we want, except that the option within the drawing for reference parts to behave like parts should actually means it behaves like parts... margins, hidden lines, sectioning, everythiing exepct appearing in the BOM / Parts List / Balloons.

So maybe a new option, leave the existing functionallity but a new "super" option that forces Inventor to treat reference data just like regular non-reference data, at least when it comes to drawing views.

Mike

[SteveMDennis]

Mike,

 The option "as Part" is only for the aesthetic look, nothing else. Just like As reference is too.  These are visual appearance options.  Making the change you suggest would be a bigger undertaking with wider ramifications.

Thanks for the discussion

[p.rybar]

Any progress in sectioning reference parts? We use them to locate smaller assemblies in the large ones and the crosshatch would be perfect for our production (we print drawings only B&W)