Whenever we design cast parts we always leave about .125" machine stock. We first create a cast part, insert the casting as the base feature in a new part and "machine" off the stock. Is it possible to show the machined state of the part in a drawing with the original machine stock from the casting shown as hidden lines or something? I've seen lots of old hand drawings done this way and it really helps the shop see what is going on. I've never figured out how to do it in SW.
Thanks
Personally, you should not be adding the casting to the machined part drawing, except as a reference only. They should have seperate part numbers or seen and controlled as seperate part drawings.
Otherwise, you can do two things: A configuration with everything suppressed except the base part. And, add the casting part into the machine drawing. (again, that is wrong, imho)
Here's an example..
We do have separate PNs and files (model and drawing) for the cast part and for the machined part. What I was wanting to do is have the original base part outline in phantom so that one could look at the machine drawing and see quickly where the stock is and isn't. The controlling document for the casting would still be the casting drawing.
thanks.
I think you will need to make an assembly of the cast model positioned coicident to a machined model. You would then make your drawing of this assembly, rather than either of the components. In each view, you can config the casting component with a phantom or whatever line font. All the lines except the machined areas will be covered up by the visible lines of the machined component. If the drawing is of a single component, you would not have any BOM problems, since no BOM is needed.
HTH bill allemann
Bill,
Another method to accomplish what you have outlined below is to use the Alternate Position view. The alternate position view that is super-imposed on the original view will automatically be set to phantom line display. You would have to create your "Cast Part" and "Machined Part" configurations ahead of time.
I've used it a couple of times and it seems to work really well for an application such as this.
Best Regards,
Ricky Jordan
Insert a view of each part in the drawing. Change the line font of the casting view to phantom. Right click the phantom view, select 'Alignment' and then use 'A;lign Horizontal By Origin'. Repeat with 'Align Vertical By Origin'.
I use this method alot when creating drawings of modified purchased parts, such as a gear whose hub is cut off.
Jim S.
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