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How to Chamfer Up to an Edge or Vertex

Question asked by Andrew Glick on Apr 29, 2019
Latest reply on May 1, 2019 by Jeremiah Feist

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Often times I have found myself working on a part and wanting to chamfer an edge up to another edge/vertex. I know I did something similar to this when using Creo, but I can't figure out how to easily do it in Solidworks. I have attached a picture of a basic sample part. Is there an easy way to bring the chamfer up to the selected edge?

On a semi-related note, I know I have seen a flip direction checkbox under the "chamfer parameters" menu when creating a distance-distance chamfer. Is that option hidden, or did I just imagine it?

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Kevin Chandler May 1, 2019 12:47 PM
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Andrew Glick wrote:

Often times I have found myself working on a part and wanting to chamfer an edge up to another edge/vertex. I know I did something similar to this when using Creo, but I can't figure out how to easily do it in Solidworks. I have attached a picture of a basic sample part. Is there an easy way to bring the chamfer up to the selected edge?
On a semi-related note, I know I have seen a flip direction checkbox under the "chamfer parameters" menu when creating a distance-distance chamfer. Is that option hidden, or did I just imagine it?
Hello,

For Q1: you'll probably have to use equations to do the math for the chamfer size.
See Mr. Edwards' reply below.

Q2: Click the little purple arrow to toggle the chamfer direction.
See Mr. Feist's reply way below.
Kevin
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John Pesaturo Apr 30, 2019 7:22 AM
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Andrew, I don't believe this is something that SW can do as specified. There's simply no option that allows the chamfer tool to behave that way. Barring sketching in your own extrude-cut/extrude-boss to create the feature in question I do not believe it can be done.
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Rob Edwards Apr 30, 2019 8:10 AM
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Hi Andrew
I don't use the built in chamfer much but think you are looking for Hold Line?

..and playing around you can add both edges
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- Kevin Chandler @ Rob Edwards on Apr 30, 2019 8:23 AM
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  Rob Edwards wrote:
  
  Hi Andrew
  I don't use the built in chamfer much but think you are looking for Hold Line?
  
  ..and playing around you can add both edges
  
  Rob Edwards Thank You
  I had forgotten about the hold line option.
  I haven't had an occasion to use it myself, but I had encountered it in a training video.
  
  Kevin
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- Andrew Glick @ Rob Edwards on Apr 30, 2019 3:58 PM
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  Thanks Rob! I'm sure this will come in handy.
  
  Do you know if that method can chamfer multiple edges in a single feature? Can you have one side of the chamfer go up to an edge and have the other side be a user-give distance (i.e. 2.50 mm)?
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  - Rob Edwards @ Andrew Glick on May 1, 2019 2:35 AM
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    Hi Andrew
    I don't think so..
    Looking in the help file it seems hold line can do some crazy stuff
    I would do as Kevin Chandler suggested and use equations, then you have complete control
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- John Pesaturo @ Rob Edwards on Apr 30, 2019 3:33 PM
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  Dang Rob ... Good find
  
  I have to say that I have never seen that before, ever ...
  
  Learn something new today ...
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- Kevin Chandler @ Rob Edwards on May 1, 2019 8:10 AM
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  Rob Edwards wrote:
  
  Hi Andrew
  I don't use the built in chamfer much but think you are looking for Hold Line?
  
  BTW: Hold line is also available for fillets (but for face fillet only):
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  - Jesse Robbers @ Kevin Chandler on May 1, 2019 11:11 AM
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    I was aware of hold line for fillet, it's useful when you want a full round on something but are only modeling 1/2 of it which is to be mirrored later on. Didn't know or trip over this yet for chamfer, like that double curved hold line type, getting into some loft/boundry type fill conditions, maybe with some new option or benefit??? Have to test it out and check the behavior thru some different conditions.
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    - Jesse Robbers @ Jesse Robbers on May 1, 2019 12:28 PM
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      It looks like, using that curvy split line image in Rob's post that using only 1 of the curvy edges as the hold line in a face chamfer acts the same, but in 2 ways depending how you look at it.
      
      One way is it acts like a lazy man type of sweep feature. The curvy edge is the path, the profile is a 45deg angle as it follows the path, the "profile" extends up to the 2 external surfaces it will intersect with. If a sweep was used, the profile may intersect and fail, or you re-size it as the path changes to make sure the swept surface is not stepped or jagged at the end due to the profile being too small in some conditions. The angle at 45deg seems to be fixed, I did not see any way to change the angle, would be nice if this was an option.
      
      The other way is to think of the curvy edge as one side of the sketch profile of an extrude cut, which is 45deg normal to the external surface. Saves time in this case as don't need 45deg normal to plane for the cut, or a 45deg path for a swept cut in this orientation. Again, a lazy man swept cut, or lazy man extrude-cut, fixed to 45deg though, would be nice to be able to change this angle, I don't see how. Lazy man in these conditions can be good, fast, stable if the intent is correct.
      
      If 2 curvy edges are used, one on each external surface, it's a little more simple or lazy man than the set up work required to do a loft/boundary cut with closed profiles, swept cut, extrude cut, or surface with a cut with surface and a delete surface body type function. Ends up the same or similar to a loft/boundary type condition between 2 profiles, just more simple or lazy man style. I didn't look close enough to see if loft, boundary, or fill is an exact or best match to this for surface curvature or anything of that nature.
      
      Doing the above actions towards a face fillet with hold line, using those 1-2 curvy split line edges isn't as robust as the chamfer function. Only 1 curvy edge can be used, to give some varying size or depth fillet that the curvature doesn't change as much throughout it's surface. I think if you want some 2 direction curvy edge type fillet function that it's better to do the leg work and complete the task with some surface fill functions after defining the boundary but the curvature may end up varying more throughout it's surface. This is more preference or application driven for which is the better choice.
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Andrew Glick May 1, 2019 11:49 AM
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After messing around I also figured out how to use a perpendicular reference sketch and figured I'd share that here. It's a bit more customizable than a "Hold Line" chamfer, but does require an additional sketch.
After sketching lines perpendicular to the desired chamfer, create driven dimensions.
You can then reference the driven dimensions in the chamfer with "D1@Sketch3" substituting for the desired dimension and sketch names.
It gives a bit more control for those of you who want it.

I know I asked this already, but I don't see the purple arrow--Is it possible to change the which side of the Distance/Distance chamfer corresponds to D1 and D2 and if you can customize it on a per-edge basis like you can with the Distance/Angle fillets? I could have sworn that was something you could do, but I cannot figure out how to do it again for the life of me!
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- Jeremiah Feist @ Andrew Glick on May 1, 2019 12:43 PM
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  Yeah, i don't see it on the distance-distance type chamfer either.
  
  but if you select the distance chamfer, and the asymmetric option, the property manager has a flip direction option.
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How to Chamfer Up to an Edge or Vertex

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