Welcome to the Onshape forum! Ask questions and join in the discussions about everything Onshape.

First time visiting? Here are some places to start:
  1. Looking for a certain topic? Check out the categories filter or use Search (upper right).
  2. Need support? Ask a question to our Community Support category.
  3. Please submit support tickets for bugs but you can request improvements in the Product Feedback category.
  4. Be respectful, on topic and if you see a problem, Flag it.

If you would like to contact our Community Manager personally, feel free to send a private message or an email.

How can I stop a Fillet from going too far along a part?

john_smith077
john_smith077 Posts: 175 ✭✭✭
edited July 2016 in Community Support
Hello

I have a problem. I want to stop a Fillet from going too far.

I suspect that the problem is that I Extruded too much at once(!) And now when I come to Fillet I need to find a way to stop the fillet.
At present, if I select one small edge at the far end of my part and then when I apply the fillet, the entire side of the part gets filleted at once!

In this case I want area C. and D. to be filleted but not areas A. and B. :



The only way I that I found whereby I could achieve this was to extrude areas "A." and "B." on a temporary basis as this seems to put the filleting off(!). And then extrude using remove back to where it was.

Although this does seem to work... is there not a better way? e.g. Is there any way you can just draw on the part to stop the Fillet from going any further?



Many thanks

J







Answers

  • brucebartlett
    brucebartlett Posts: 2,148 PRO
    Hey John, If you share a public doc url (copy and paste from the browser) we can take a closer look. 


    Engineer ı Product Designer ı Onshape Consulting Partner
    Twitter: @onshapetricks  & @babart1977   
  • jakeramsley
    jakeramsley Posts: 669 image
    It's possible it is tangent propagation.  With that option on, fillet looks for edges that are tangent to it and applies the same fillet to it.
    Jake Ramsley

    Director of Quality Engineering & Release Manager              onshape.com
  • john_smith077
    john_smith077 Posts: 175 ✭✭✭
    I've made rather a mess of the document since posting the above but here is another example problem (in the same document)



    As you say if "Tangent Propagation" is switched on, it fillets the big circle below it. 
    But if I dont have Tangent Propagation switched on then it doesnt seem to fillet at all !

    Fwiw, my cunning scheme to apply an extrusion where I want the propagation to stop isn't very clever because it wont let me Extrude with Remove back to where it started !

    Anyhow here is the URL 
    https://cad.onshape.com/documents/f08cf9fe372f41b5a331512f/w/dd46f3348064476e8acbba79/e/416c3409f0f44a95a6ec2383
    Which I can leave public for 3 days or so only. 

    In this case there would be other ways to remove the material (e.g. with an Extrude Remove) but in other situations doing a partial fillet it may not be so easy...(!)

    Many thanks





  • jakeramsley
    jakeramsley Posts: 669 image
    If you want to have it end at that point, I would do a sweep -> remove with the section you want to remove.

    1. Sketch on the end face and draw an arc and two lines creating an enclosure.  Set the lines coincident with the edge and their shared vertex coincident with the end vertex.  Then set the arc to be tangent to both edges.  Add a dimension for what the value of fillet you want.


    2. Start a sweep.  Select the sketch profile as the profile to sweep and then pick the edge for the path.  Set the type to be remove.

    Jake Ramsley

    Director of Quality Engineering & Release Manager              onshape.com
  • 3dcad
    3dcad Posts: 2,482 PRO
    john_smith077 said:
    ..

    Fwiw, my cunning scheme to apply an extrusion where I want the propagation to stop isn't very clever because it wont let me Extrude with Remove back to where it started !

    ..

    On depth defining to fillet I agree with Jake.

    For your workaround I would use 'move face' so that first move say 20mm out then same value back in. If you wan't high end, create a variable and use that as value for both directions. 
    //rami

Categories