Chamfer edges of square hole

[cmarinelli]

The problem I'm about to describe sounds like it should be easy to resolve, but has me dumbfounded.

I have a rectangular hole in a plate with a radius (not full) forming one side of the rectangular hole. There is a .025 chamfer on three edges of the hole. The intersecting chamfers have a .040 radius, and the two ends of the chamfer also have a .040 radius. When you chamfer the edges, you get a sharp corner where the chamfers intersect. This of course, does not reflect what actually occurs when you use a conical form tool to machine the chamfers. Additionally, when you chamfer the edge intersecting the unchamfered edge, you get a sharp end to the chamfer, whereas in reality you obtain a conical surface at the end of the chamfer.

I've tried doing a cut-sweep which does fine on the right angle edges to be chamfered, but leaves a vestigial post or boss at the center of the .040 R at the end of the chamfer. The sweep cut command fails if I enlarge the profile to try to eliminate the post because the sweep profile interferes with itself.

Is a sweep cut the best way to do this?

Is it possible to create a 'form tool' with a 90 degree tip and conical ends? This form tool could then cut this shape out of the part.

Does anyone have a better idea?

Thanks in advance,
Chris Marinelli
Dynatech Engineering

 

[macPT]

cmarinelli

I don't understand the problem you are describing. You are refering a chanfer and then a radius: do you mean a fillet?.

If you mean a chanfer, you can chanfer the edges and then a fillet in each of the corners (I think the geometry is correct).

If you mean a fillet, I think a sweep cut is the way to go, but you should try some solutions because it will not be easy (I think, in the "real world", you will never have a smooth transition in the corners, with a square hole and a conic tool).

Regards

 

[mncad]

cmarinelli,

I think what you want to do is possible. You will have to determine the diameter of the cutter at the top of the chamfer. Then sketch the outside profile of the cutter path using the diameter of the cutter as the radius in your corners. Then use the extrude cut command with the draft set at 45 (or whatever angle your chamfer is) when you make the cut. Guess I'm assuming that your cutter is small in diameter compared to the size of the square hole and will be running a path to achieve the chamfer.

mncaad

 

[SBaugh]

I'm not sure what you’re trying to describe exactly either, but have you tried a face-to-face fillet, or tried picking the intersecting corner between chamfers.

When trying your sweep, your sketch profile maybe to big "hence" the error interferes with itself. Make the profile smaller and then make a second sweep if necessary.

Regards, Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.3dmca.com

faq731-376
When in doubt, always check the help

 

[cmarinelli]

I think mncad has come up with a viable solution. Thanks a lot. I'm going with this for now.

I re-read my problem description, and I can see why everyone is confused. To re-phrase, I would essentially like to extrude-cut a cone through the solid, much like an end-mill with a pointed tip would cut through material. It is basically a v-notch with a cone at both ends.

Using mncad's solution, you can extrude-cut a slot with a 45 degree draft angle, but the depth can't equal the width or else it comes to a point (which is actually desirable).

Is there a way to take a solid (e.g. drill shape or other form tool), and then extrude cut along a path through another solid? Sweeps only work with 2D profiles, and lofts don't seem to work either. Any ideas?

 

[sirmick]

Wouldn't a revolved cut give you the results you want?

 

[SBaugh]

It isn't going to matter you going to have to use a 2D sketch whether its sweep or a loft.

With a loft you can use a 2d profile and a point x distance away from the first sketch then place a guide curve in between the 2 and use a cut-loft.
Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.3dmca.com

faq731-376
When in doubt, always check the help

 

[mncad]

cmarinelli,

You didn't say in either of your posts which version of SW you are using. If you are using SW2003 you can use the multiple bodies to do what you are asking. Its not a perfect setup but you can come reltively close. The way I have worked it is to model the path of the cutter, be sure when you do the extrude of the cutter to click off the button that says "merge results" in the extrude window. You will now have to solid bodies, your part and a model of the cutter path. Then in the menus click "inserts", "feature", "combine". When the combine window comes up it will give you a choice of add, subtract and common. You want to use the subtract command. Then pick your part as the base and the model of the cutter path as what to remove. Like I said, it's not a perfect solution but works pretty well. You can have the same issues as you pointed out before with the profiile trying to come back on itself.

mncad

 

[skiking]

If you will send me your email address I will send you a sample that you can look at that will show a rectangle hole without radius corners and one with radius corners and what happens when you chamfer the edges. My email address is jradney@coastalind.com

 

[WDickman]

I think this is one solution to the problem. First create the square hole in a part. Then "loop select" the 4 top edges of the hole. Now you have a square hole with a chamfer all around. The problem now is you have 4 sharp inside corners. Not easy to do with a 45 degree mill cutter. Now you want to fillet these 4 corners using the variable fillet tools. Decide what the smaller fillet radius will be, (at the bottom of the existing chamfer) & calculate the top fillet radius that you get by using a 45 degree cutter. This should give you a chamfered hole as if you chamfered using a 45 degree cutter. Confusing? Certainly!

 

[WDickman]

Oops! After "loop selecting" you want to chamfer the hole with your favorite chamfer size. Then go to filleting.