Casting Parts using part copy function 1

[QSubs]

I am designing a number of cast parts using the part copy feature. I model the casting then part copy this part into a new file then cut away the machined surfaces that are required.

When i go to draft the component i specify the material as the casting part number.. Is there any way to do an auto call out to call up the document number of the part that has been part copied?

Thanks

Andrew

 

[KENAT]

I think so, if using a 'call out' click the property text button bottom left in the pop up window & select 'named reference', double click the properties you want to display then OK.

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[QSubs]

mm Ive had a look in there but i cant find anything to link to the copy part file name..

 

[bshand]

QSubs,
That's an interesting problem. I can't find any way to link to the interpart linked file. I assume you are in ordered and the copied part is linked. The only workaround I can think of is to type it into an existing or new property and reference that in the callout. This would be a good post in the Siemens SE forum:

http://community.plm.automation.siemens.com/t5/Solid-Edge-Forum/bd-p/solid-edge-forum

I may ask it if you don't and you don't mind.
Bruce

 

[KENAT]

Hmm, I just tried an you're correct, sorry.

One possible work around, temporarily add a view on the drawing of the cast part i.e. fed by the cast model.

This should allow you to use the property text technique I mention.

You should then be able to delete the drawing view and keep the property text linked to that model.

May have issues maintaining links if you move/rename files but might work.

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[KENAT]

Oh, and of course it's not truely intelligent. For example if you change the cast model being used as the base point, this call out will not update to the new model..

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[bshand]

Kenat,
Nice. That does seem to work for a callout. If you need it in a BOM I think it won't work.

 

[KENAT]

Well, for a BOM you could create a dummy assembly with it in etc. but again, it's a kludge.

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[bshand]

Yeah, you might as well type it in directly or into a property. It seems odd that there's no way to link to an interlinked part. The software obviously knows it's there they just need to provide a hook.

 

[ct27gt]

^^ Creating a custom property would be a good workaround method here.

The only other way I could think of is put in the view as KENAT mentioned, but don't delete it, put it on a hidden layer. This way it can stay in the drawing. This will be a good indicator if you go to do another drawing, you realize the number is wrong. Since its paramentric to the model, this would tell you that you need to insert a different model. Its also nice, because then the reference to the casting model shows up when looking at links.

I would recommend this if you are the only one working with the models. It could be confusing if someone else tried to work with your model. Its still the most parametric way to do it that I can think of. Just name your layer something descriptive like "HIDDEN CASTING MODEL VIEW".

 

[bshand]

You can't hide a view that way. You'd have to put it outside the sheet boundary so it doesn't print.
As to it being confusing, if that's the accepted methodolody within a design group then no problem.

 

[ct27gt]

Not true. I just put a view on a hidden layer and it works. I am using ST7, maybe its different in earlier versions?

 

[QSubs]

bshand
Sure you can post on the other forum, any help would be great.

Its strange that there isn't a simple way of doing this. There is functions and call outs for almost everything else. Its there a different way do design casting components with making the casting part and machined parts linked?

I don't want to keep manually putting the information in as sometimes the revision changes of the casting and it would be really nice to be able to update the draft with the casting revision updating also.

Thanks

Andrew

 

[bshand]

"Not true. I just put a view on a hidden layer and it works."
Son of a Gun!

 

[bshand]

The only way I can think of doing it is putting the casting in an assembly (a single part assembly obviously) and apply machining features as assembly features. That's how I've seen casting/machining and weldment/machining documentation done when it is necessary to keep the steps as discrete operations. There's no downside as you're already creating two files with a part copy. And the assembly will give you some good BOM options as well as callouts.
And it's intelligently linked so it will automatically update and be obvious to other users how it's structured. Actually it probably is the best way to do it.

 

[KENAT]

Yeah, bshand's approach is probably the best one and I'm not sure I can think of an obvious problem. Are all the part feature types available as assembly features - I don't use that functionality much.

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[bshand]

Kenat,
Since it's a machining you just need to remove material and all the machining features like cuts and holes are available. IOW things that remove material. You could even add studs, thread inserts, etc. as items in the assembly if needed.