Is there an easy way to chamfer part of an edge?
I needed to chamfer 52mm of a 56mm straight edge but only had the option of chamfering it all using "chamfer".
In the end I had to create a new plane using that edge and cut the chamfer out.
Better to shoot an image for better understanding
you can use extrude cut option, with 52mm and required angle
You do not have the option to use the Chamfer with a fixed length, i.e chamfer for 52mm.
You will have to do as Denny suggested and create a sketch (chamfer profile) on the end of you plate and cut extrude for the length.
I do this quiet often and its a right pain (more work), I am sure I brought this up years ago and am still waiting for this ability.
See attached for another way of doing it.
An image of the same please
I just used the split function to create an edge to chamfer to, then used combine to join the two bodies together again. Might not be able to do this in some cases, but a useful technique nonetheless.
i dont have access to SW rit now, thats why asked an image
here you go, a step by step.
Good job Greg
Direct extrude cut is the easiest one i believe , beacuse this will take much time when compared to a blind cut
I agree, but sometimes you cant do a blind cut, because the edge isn't straight or some other issue, use it a lot on curved edges.
Sometimes, depends on the part complexity
If the edge isn't straight, use a sweep cut.
Most of us use "Sweep Cut" for that, but creating the path/guide line to specific start/stop points and beginning or ending the cut at specific angles or blends remains very complicated and requires many steps. It could more easily be a sweep this cut "from here-to-there" and end square to cut or surface or at an angle to cut or surface or blend to original faces. That would be a big improvement in the sweep, fillet and chamfer commands.
I had seen some people adding material at the end after a through chamfer, part looks the same but not the right way to deisgn it.
This issue has come up quite a lot in what I do. I have used all of the solution methods described by posters, which can be lengthy and involved, but would LOVE for SW to make a Chamfer or Fillet "to here" feature, with an option to end square or blended into the original surface(s). I had that capability way back in the early 1990s with Solution 3000. All we had to do was add a construction line or plane to the model where we wanted the feature end, et voila!. Hey Solidworks, this capability doesn't seem like algorithmic rocket science, get on this will ya please.
Submit it as an idea to the SWW2015 Top 10 Ideas.
I do both radii and chamfers to a depth often enough that I've created library features to do it. Drag and drop on the face, edit sizes, done.
I am an industrial designer always working on something completely different than the last thing - often with spline curves and Boolean surfaces. I often need a sweep path to follow odd curves and splines, etc. Correct me if I am mistaken, but a "to a depth" library feature would not work in my situation.
My first thought would be to agree with you and say no. But on further reflection, I'm not so certain. I'm wondering why you couldn't use the library feature to create the sketch on the surface (the driven sketch), and then select a pre-existing sketch along a swept edge (offset the edge, and drag an end back to where you want it). Might work.
Well, it works. I thought that you'd have to create the sketch to sweep along before inserting the library feature, but no, the feature creates it. Kinda cool actually. I know that this is pretty simplified, but maybe you could take it as a start and develop it from here. This is the resulting chamfer on the swept edge. BTW, it only works on a single edge, not a chain of edges.
Often there is no pre-existing surface to create the sketch or path on (per se), to create the driven sketch I have to add a cut plane on which to draw it and then convert bits of surface edges into path lines onto a second cut plane. Then there's the issue of blending the ends of the partial sweep back into the original faces, which involves extending the guide path out into space, adding a revolve cut or various fillets/rounds. If a library feature can do that, I'd like to see it.
I'd like to see it too. But that doesn't mean that it can't be done. As far as needing a pre-existing surface for the path, that should be an edge. If you don't have a pre-existing egde, I don't see how any chamfer would work. You don't need a plane or face to put the profile on. The library feature can create that as well. All you need is an edge (and it's endpoint, which by definition, it has to have). Blending the ends back into the original faces really ins't part of the chamfer, I don't think. That's a blend, and there is a tool for that.
The original poster is trying to create a partial chamfer as you did, that's true, but other posters since then got into partial sweeps. I sort of inadvertently started a new thread. I have to create cuts and additions of unusual shapes along even more unusual solids.
Getting back to this topic, I used to use a program that could do what you did and asked how you wanted the end blended in the original command, no extra steps. It's also more difficult if the chamfer (or whatever cut/sweep you're using both begins and ends in the middle of the part and reaches neither end).
Yes, starting in the middle is tougher. A sweep in SW cannot go in both directions, making this pretty impossible.
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