Enclosed chamfer 5

[hititfaster]

I'm designing a part that will be milled from aluminium. I want to specify a chamfer feature but do not want it to run the entire length of the edge it will be placed on. I don't know what this might be called, and I haven't managed to get exactly what I'm looking for by searching, but I have modelled it by making an extruded cut in a 45º shape, then using a revolved cut each end to simulate the 45º mill cutter.

This does give the result I want, but it just feels a bit 'clunky' and requires several processes to complete. Is there a better way?

 

[Gupta65]

I guess you're already using one of the method. The other option might be a sweep cut.

In case you need this feature again and again, I would suggest you to create library features based on the need and use them instead.

Deepak Gupta
CSWE, CSWP, CSDA
SW 2011 SP5.0 & 2012 SP3.0
Boxer's SolidWorks™ Blog

 

[Jboggs]

Sometimes the best way to model things in SW is to think like a machinist. How will they cut your feature? They will turn their cutter on a 45 degree angle and proceed with the cut. Visualize the axis of the cutter. Turn your part on its side, looking along the chamfer length. Draw a sketch in that plane with a centerline at the angle of the cutter axis (45 degree). Create a plane perpendicular to that line. Start a sketch on that plane. You are now looking down along the axis of the cutter at that point. You can draw the full outline of the cutter path, probably a slot shape, and extrude cut it. That gives you the chamfer AND the cylindrical cutter exits at both ends, all in one extrude cut.

 

[hititfaster]

Jboggs - Interesting: I like that approach. I have been doing my best to think like a machinist (few years since I used a mill!) and so far it has been reasonably successful. I hadn't considered that you might rotate the mill head to 45º, rather I thought you would use a 45º cutter and keep the head vertical.

A setting under the chamfer tool that lets you back the chamfer away from an edge and apply a start/end detail like this would be fantastic!

 

[mncad]

On a plane perpendicular to what jboggs suggested at the depth of the chamfer, sketch a slot that is the root diameter of a 45 degree cutter and then cut extrude and apply an outward draft at 45 deg. You could also do a Swept Cut Solid. Create a solid revolve of your milling cutter, whether a straight mill or 45 chamfer mill, click off the "Merge" radio button when you revolve. then sketch the path to follow, then use the sweep cut command, at the top of that pick "Solid sweep". I have attached a part showing 3 of the ways I think work pretty well.

mncad

 

[mncad]

hit enter to quick, didn't get the file added. This is SW2010

 

[mncad]

Thought of 1 more way, 1 feature for both chamfers. You might have to do calculation for your depth. The part is attached. As jboggs said, it all depends on how it will be fixtured and machined.

 

[Updraft]

Unless you have very specific reason to make a feature a certain way you should just define what you want, include what is allowable, and let the machinist figure out the best way. For instance, will it be easier for the machinist to turn the part or the head and use a standard endmill? If using a standard endmill and expecting a circular runout then you should define a range of cutter diameters that are suitable; allowing the machinist to use a standard cutter should also allow him to use one he already will be using to make the part. Will it be easier to use a bevel cutter that he already has loaded for cutting chamfers? That is our standard method, and even then it has a runout so we model that to know what we are getting on the part.

If what you want is a chamfer to go part of the way along the edge then specify that. This CAN be machined without a runout, but if a runout is allowed then indicate how much you can tolerate such as "R.500 Max Runout Allowed". Many designers unwittingly add cost to a part by over-specifying details or manufacturing methods that do not affect the part's function. It is good to think like a machinist so that you can be sure the part CAN be machined, but if that is not your wheelhouse then effectively specifying machining methods tends to cost money. For instance, rotating the part (using a fourth axis) or the head is considered an additional setup, but a tool change to swap to a bevel cutter is very fast.

When in doubt, talk to the machinist and let him know what you are after and ask how he would approach it. Then you are in a better position to specify the right things on the print.

- - -Updraft

 

[ArtL]

Hititfaster - You are correct!!! The other options suggested,need the part or head / spindle to be moved.Not a really good idea if cost is a factor. Yhe only thing I would change is don't make the "inverted cones" at the end of the chamfer to come to a sharp point.center cutting with a 45 deg cutter usually is not a good idea, no chip clearence close to the point.Ie: if you are cutting a 1/4" chamfer the toolpath offset from the part would be .3". That way no center cutting and a clean chamfer,also the on move in and exit will be a upside down truncated cone.Sorry I don't really know a easy way to display this.I usually cut - extrude chamfer and swing,rotate cone from the side faces left after cut extruding chamfer

 

[ArtL]

Mr, Hitit Offset would be.150" - sorry about that.

 

[hititfaster]

ArtL - good to hear I'm doing something right! I was a bit lazy with the inverted cones: the cut extrude left a triangular face at its' end, so I created a sketch on it, did convert entities to grab the entire outline then used the vertical line as the axis of rotation.

Updraft - I was wondering how to specify the allowable runout, so you have answered my question perfectly. I will be adding that to my drawing in due course.

mncad - I like the extruded slot method. I have to say, the third one though, using a solid and removing material... Would never have thought of that! I'll keep that in reserve for future use!

Have a star, the lot of yer. Very useful, thanks.

 

[hititfaster]

ArtL - I am a.) English and b.) 26 years old, so I don't understand you funky imperial dimensions anyway

Just kidding - I like your attention to detail. Thanks!

 

[ArtL]

Mr Faster Being 2 1/2 times your age, metrics are new to me!!! I used imperial because I don't need a cheat sheet to know what fractions transpose to. Have a good day!!!

 

[mjcole]

SolidWorks has a sweep solid body option that can be used to sweep a separate Solid Body that is used as the cutter. You can use a partial length curve like you mentioned with the Convert Entities command or split the faces to make a smaller edge.

In regard to the Imperial system, I much prefer Imperial Ales to Imperial Dimensions.

"It's not the size of the Forum that matters, It's the Quality of the Posts"

Michael Cole
Boston, MA
CSWP, CSWI, CSWTS
Follow me on !w¡#$%
@ TrajPar - @ mcSldWrx2008
= ProE = SolidWorks

 

[mjcole]

Here's the image showing the Solid Sweep option I posted yesterday. I did not have time to post it yesterday in my original message.

"It's not the size of the Forum that matters, It's the Quality of the Posts"

Michael Cole
Boston, MA
CSWP, CSWI, CSWTS
Follow me on !w¡#$%
@ TrajPar - @ mcSldWrx2008
= ProE = SolidWorks