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Fillet-Two Surfaces or Fillet-Three Surfaces to add material near drafted features?
christopher_owens
Member Posts: 235 ✭✭
I created a simple model to show what I was wanting to do. I had two drafted surfaces that ended up forming a flattened V. I wanted to add some material in the valley by creating a fillet between the surfaces. Didn't see that option under Fillet. So I created a sketch (where you can create a fillet in the V sketched lines) and did an Extrude-Add. Easy enough to do in the simple model. Any thoughts on filling in a \-/ shape? I did try a Move Face on the actual model but that moved the entire face where I didn't want to increase the wall thickness. Guess I could do some Boolean caulking!
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Best Answers
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Currently Onshape cannot add a fillet that would blend between the side faces to create the full round. I'll add you to that improvement ticket.
You can remove the bottom of the \-/ by using delete face and then filleting the resulting single edge. See my example file using remove face and fillet.Andy Morris / Head of Product Design / Onshape, Inc.5 -
By re-ordering the fillet features to after the shell its easier to control how the radii on the internal faces work. You can also remove the slither faces and thin cuts by using a replace face to butt one face against its neighbor, though this will change the wall thickness slightly in certain areas.
Andy Morris / Head of Product Design / Onshape, Inc.5
Answers
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Made a quick test. Seems to work fine with sharp corner, but with flattened V result will be different.
I would do final shape directly in sketch or make flat V line construction figure and extend to sharp V to be able to fillet only one the bottom line.
//rami0 -
Currently Onshape cannot add a fillet that would blend between the side faces to create the full round. I'll add you to that improvement ticket.
You can remove the bottom of the \-/ by using delete face and then filleting the resulting single edge. See my example file using remove face and fillet.Andy Morris / Head of Product Design / Onshape, Inc.5 -
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On the above green sample part it didn't work, I assume because the V extended outside the part. But on the "real" part I did the 'Remove Face-Cap Void'
and it retained the wall thinkness for the entire face! As you can see in the image the face extended beyond the V. Without the 'Cap Void' there was an opening where the face and wall use to be.
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I may of gotten excited to soon! Upon further review, there still was a \_/ that must be due to the 'Shell' thickness of 1mm. As I play with that value you can imagine the \_/ gets larger or becomes a V. I don't have professional experience with drafted plastic parts (shows eh?) but the CadCrowd contest I am doing this for wants a 3D Printed prototype but with all the drafts required for injection molding. I figure a molding tool isn't machined to a sharp point so that is why I am adding "rounds". Molded parts gurus out there??
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By re-ordering the fillet features to after the shell its easier to control how the radii on the internal faces work. You can also remove the slither faces and thin cuts by using a replace face to butt one face against its neighbor, though this will change the wall thickness slightly in certain areas.
Andy Morris / Head of Product Design / Onshape, Inc.5 -
@andy_morris Thanks! You can image as I modify the design (moving features around), all this changes! I also thought of leaving all the radii in the model to last. Stop trying to make the model "look pretty" and get a final design for the customer to see! The 3D Printing will "round" the edges anyway. Let the people that make the actual mold work their magic! I don't know if they would even use my model anyway. Kinda like putting bend allowances in a sheet metal model. Every supplier likes using their own "formula".0
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Any update on the feature for the fillet to be able to blend surfaces? that would be super useful2
