I have a roller that needs to have draft added to both ends, so parting line is in the center of the bore. Can someone walk we through the process.
Create two holes with draft ... one from each side, or use a revolve which includes the 'draft', or create one half of the roller and then mirror.
That's the simplest
Or put a Split Line where you want the opposing drafts to meet and then add two Draft features, one for each direction.
I had several failed goes at this. The split face shows up but the draft did not generate. Can you look at my model ! and see where I messed up.
I'm still running SW2010 so I can't open your file. I can't remember ever having the Draft feature fail in a simple case like this seems to be. Sometimes the results aren't what I would like when the parting line is more complicated or I've got different draft values on the two side. Does the Draft feature give you an error message or does it just fail quietly? (Just desperately searching for clues.)
When I create the draft both neutral face and the draft plane show up on the graphic, but check OK and no draft is generated. No error message just fails quietly.
Much appreciate you trying to help
Using your model I have created a split line in the center of the bore in line with the front plane. ( I have cut you model in half to make it easier to see what I am doing in the pictures)
I then added the draft using the Front plane as the neutral plane, I then selected one of the inner faces.
You can see the resulting draft below
If you want the draft to go in the opposite direction select the flip direction box and the direction arrow will flip direction
If you need to used one of the end faces as a neutral plane first split your part into 2 pieces using the split command (insert - features - split )
then using the draft command you can select one of the end faces as the neutral plane
You will then end up with this
Then draft the other end
Now use the combine (insert - features - combine) to merge the 2 bodies back into one part
Hope this helps
Perfect! I was using and end face not the Front Plane for the Neutral Plane.
Much appreciate your help
here is a simple way with only a cut using the your first sketch
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