Milling Chamfers

athack · Apr 10, 2013

What is the most common programing method for milling a chamfer with a chamfer mill? The two I am interested in are pocket milling circles and odd shapes. We are having trouble and seem like it takes too long to program.

Thank You

Athack

Hertz · Apr 10, 2013

I use Mastercam. Toolpath contour, select profile, select chamfer in parameters. Done.

dandrummerman21 · Apr 10, 2013

Determine the diameter of the chamfer tool at an arbitrary depth (For this example, lets say .100" from the tool tip). If you want a .04" chamfer around your part, make your CAM program contour around the part at a depth of .140", and use the diameter than you measured at .100" as the tool diameter.

That example is assuming a 45* chamfer.

Alternatively, you could draw an offset line/shape that is the same distance away from your shape as your chamfer is specified, and use the diameter of the tool at .100" to contour the new shape at a depth of .100"

Either way works. Hope I explained it well.

jeuhrn · Apr 10, 2013

Most chamfer mills are 90 degree, and they have a flat spot on the end. One I use is marked ø6/ø1 meaning it has a ø1mm flat spot on the tip, and it's ø6mm at the largest. If you are good at math, or have a CAD program you can draw up the shape and see what diameter the chamfer mill has at different depths. If it's one of those multi-operation 90 degree angle tools (NC drill, chamfer mill, etc) that actually comes to a point, it will have a diameter of 2xDepth at any given depth.

The radius of my chamfer mill is 3mm, but I set it to 2mm in the tool list, so it'll effectively go into the material 1mm to each side whenever you're using cutter comp. Then I usually go Z-1.5mm or Z-2mm depending on how large a chamfer I want, and just follow the same contour as the I made with an end-mill previously.

Practical example:

T1 M6 (10MM ENDMILL)
S10000 M3
G89 X50 Y50 Z-10 K10 B2 Y5 F1500 (CANNED POCKET CYCLE)
G79 X100 Y-100 Z0
G0 Z10
T2 M6 (CHAMFER MILL)
G89 X50 Y50 Z-1.5 K1.5 B2 Y5 F1500
G79 X100 Y-100 Z0
G0 Z10 M30

John Welden · Apr 10, 2013

Surfcam has a really nice chamfer tool path feature. It pretty much figures out everything for you.... quick and easy.

Hertz · Apr 10, 2013

You guys make it complicated. No need to draw extra lines or compensate depths blah blah. If you have a decent cam package, there is no need to do anything. Its 45 degrees so whatever you put in depth, is what will be radially. Use a contour toolpath. Select your chamfer tool, put the depth in. There is no need to get technical for a simple chamfer.

dandrummerman21 · Apr 10, 2013

Not all chamfers are simple 45's, not all chamfer tools are small, not all chamfer tools have a diameter specified on the tool itsself, not everyone has a decent cam package, etc etc. I get to choose any number of ~15 different chamfer tools, depending on what tools are available vs what tools are in other machines, and the size of the chamfer. With odd angles (Why does the engineer want 38*???) it's easier to draw an offset line and get the diameter of the tool at whatever depth you plan on running the tool at, although certainly not required with some trig or trial and error. If your cam package can do this with a click of a button, good for you.

There certainly wasn't anything complicated about my method ¬_¬

Hertz · Apr 10, 2013

dandrummerman21 said:
Not all chamfers are simple 45's

Perhaps not, but the OP did not specify and the second poster mentioned most are 45 so we assume the OP is using 45. I assume anyway. Besides, the angle is not relevant.

not all chamfer tools are small

I don't get this comment? Does the size matter?

not all chamfer tools have a diameter specified on the tool itsself

Not relevant. Get your vernier out.

not everyone has a decent cam package

I have to correct my statement. If you are using a cam package.

I get to choose any number of ~15 different chamfer tools, depending on what tools are available vs what tools are in other machines, and the size of the chamfer. With odd angles (Why does the engineer want 38*???)

Draw this tool and save it. Select it when you want to do a 38 degree chamfer. Cam packages have a chamfer selection in the parameters. if you have a cam package that does not have this feature, then its junk. lol
Mastercam for example has a width and depth/tip offset parameter. if you select a 38 degree tool from your library, you enter in the width and depth/tip offset. Simple. What I'm trying to say is there is no need to draw extra geometry. Its wasted time.

it's easier to draw an offset line and get the diameter of the tool at whatever depth you plan on running the tool at

No it is not. lol The beauty is once you have that tool defined, its always there for selection and to me its easier to enter your width and depth than it is to draw extra lines. besides it makes the model and/or wireframe look dirty.

If your cam package can do this with a click of a button, good for you.

Yours does not do this? What are you using?

There certainly wasn't anything complicated about my method ¬_¬

More of a reference to you and that other guys post. I combined the statement. I'm not saying what you're doing is wrong, not by any means. Just saying there is no need for it.

dandrummerman21 · Apr 10, 2013

Gibbs. For one, it has a plugin for chamfers that seems to only work for solids (which we do none of). Moreover, when I create a chamfer tool using the tool creation dialogue, it always wants to use the max diameter of the tool I create (instead of somewhere in the middle of the chamfer). If I draw the tool properly (as in, I draw the tool's full diameter), generating a simple contour around the previously drawn line will result in nothing being cut. Simply (and by simply I mean 2 clicks) creating an offset contour works well for this.

However, I don't use that method much (hence it being the second suggestion in my post). I just throw the tool on the optical presetter, discover the diameter at a given depth, use gibbs to contour around the originally drawn line, and go deeper. It's pretty similar to your method anyway.

If there's multiple ways to chamfer a cat, and I know about them, I'll say em both. I almost didn't even feel like typing this out to defend my methods. Not productive.

DMF_TomB · Apr 10, 2013

milling chamfers can be done different ways. what i use where i want to control Z position of chamfer cutter.
.
1) use a chamfer cutter with a flat tip and measure tip diameter.

2) treat it as an end mill with end mill diameter as tip width

3) put tip corner at depth you want. as it contours it will leave a chamfer.

simple and you know exactly the tip depth of chamfer cutter (chamfer end mill) will be at. Allows chamfering where chamfer cutter tip will be within 0.005" distance of vise jaws. works with any angle. you just need to know depth of chamfer and diameter of tip of chamfer cutter.

706jim · Apr 10, 2013

One other consideration is the presence of adjacent geometry (walls above the level of the chamfer). In this case, you need to control the position of the tool to avoid accidently cutting these features. My CAM system will show interference with these adjacent features which may require offsetting the profile and/or depth of the tool as it makes the chamfer.

So, just goes to show that there are different methods of getting this job done.

Mike Ortega · Apr 10, 2013

Hertz said:
I use Mastercam. Toolpath contour, select profile, select chamfer in parameters. Done.

And done

jeuhrn · Apr 10, 2013

dandrummerman21 said:
Gibbs. For one, it has a plugin for chamfers that seems to only work for solids (which we do none of). Moreover, when I create a chamfer tool using the tool creation dialogue, it always wants to use the max diameter of the tool I create (instead of somewhere in the middle of the chamfer). If I draw the tool properly (as in, I draw the tool's full diameter), generating a simple contour around the previously drawn line will result in nothing being cut. Simply (and by simply I mean 2 clicks) creating an offset contour works well for this.

However, I don't use that method much (hence it being the second suggestion in my post). I just throw the tool on the optical presetter, discover the diameter at a given depth, use gibbs to contour around the originally drawn line, and go deeper. It's pretty similar to your method anyway.

If there's multiple ways to chamfer a cat, and I know about them, I'll say em both. I almost didn't even feel like typing this out to defend my methods. Not productive.

I also use Gibbs, but I don't use the chamfering plugin. I define the tool as a chamfer tool, and then I just use a contour path offset to the side and input -1mm in the XY stock (for a vertical mill), and a depth somewhere near the middle of the chamfer.

maz43 · Apr 10, 2013

I have no Cam system. I just use CRC and cut and paste the original profile tool path for the chamfer tool.

dylskee · Apr 10, 2013

dandrummerman21 said:
Gibbs. For one, it has a plugin for chamfers that seems to only work for solids (which we do none of). Moreover, when I create a chamfer tool using the tool creation dialogue, it always wants to use the max diameter of the tool I create (instead of somewhere in the middle of the chamfer). If I draw the tool properly (as in, I draw the tool's full diameter), generating a simple contour around the previously drawn line will result in nothing being cut. Simply (and by simply I mean 2 clicks) creating an offset contour works well for this.

However, I don't use that method much (hence it being the second suggestion in my post). I just throw the tool on the optical presetter, discover the diameter at a given depth, use gibbs to contour around the originally drawn line, and go deeper. It's pretty similar to your method anyway.

If there's multiple ways to chamfer a cat, and I know about them, I'll say em both. I almost didn't even feel like typing this out to defend my methods. Not productive.

Using Gibbs you just specify your chamfer size and give it a depth and it will create the chamfer for you. If the chamfer mill starts to wear at that point you simply change the depth and it will cut the same chamfer size at the new depth.

dandrummerman21 · Apr 10, 2013

dylskee said:
Using Gibbs you just specify your chamfer size and give it a depth and it will create the chamfer for you. If the chamfer mill starts to wear at that point you simply change the depth and it will cut the same chamfer size at the new depth.

But what does your tool look like?

Say I have created a tool that looks like this:

The largest diameter on this tool is 1.5". Small diameter is 1". When using the same parameters you have, this tool will never hit the edge with the tool I created.

That's why I get the diameter off the optical presetter. If my cut depth is .03", I'll get the diameter .03" from the tip of the tool. I can then use a negative stock value to get the desired chamfer, or simply go deeper. Either way.

I guess I forgot to mention above; the offset curve method is *very* useful if the chamfer does not go all the way around the part, and may trail off in a spot. Not run off an edge, but a constant decrease in chamfer depth or other similar feature is a good candidate for offset curve.

kootne · Apr 10, 2013

DMF_TomB, you and me think the same. works with cam or longhand. just follow the line you already followed with your profiling tool. value of -Z= champher. limited opportunities for cerebral flatulance.
kootne

christinandavid · Apr 10, 2013

I believe that Athacks question has been answered. There is no most common programming method. I am lucky to have cycles at my control (manual guide i) but if I didn't, I would probably create a macro to alter my wear offsets so i could use any point on the cutter, then run the same path as the other milling cutters.

The main issue is coming up with a standard procedure everyone agrees on and understands. There is nothing worse on a repeating job than trying to set up a chamfer mill with no information or logical process in the program.

DP

Greg White · Apr 10, 2013

Well heck I feel like commenting,
I do the horse and buggy way with G& Ms,
I put my profile in a sub,then call sub after tool call,the I can change tools and tool call, call sub,
dun.
Gw

dylskee · Apr 10, 2013

dandrummerman21 said:
But what does your tool look like?

Say I have created a tool that looks like this:

The largest diameter on this tool is 1.5". Small diameter is 1". When using the same parameters you have, this tool will never hit the edge with the tool I created.

That's why I get the diameter off the optical presetter. If my cut depth is .03", I'll get the diameter .03" from the tip of the tool. I can then use a negative stock value to get the desired chamfer, or simply go deeper. Either way.

I guess I forgot to mention above; the offset curve method is *very* useful if the chamfer does not go all the way around the part, and may trail off in a spot. Not run off an edge, but a constant decrease in chamfer depth or other similar feature is a good candidate for offset curve.

I thought we were referring to a simple 90 degree chamfer tool, I see what you're saying with a tool like that........

Milling Chamfers

Stainless

Stainless

Stainless

Plastic

Diamond

Stainless

Stainless

Stainless

Stainless

Diamond

Titanium

Aluminum

Plastic

Aluminum

Cast Iron

Attachments

Stainless

Aluminum

Aluminum

Titanium

Cast Iron

Similar threads