• Scam Alert. Members are reminded to NOT send money to buy anything. Don't buy things remote and have it shipped - go get it yourself, pay in person, and take your equipment with you. Scammers have burned people on this forum. Urgency, secrecy, excuses, selling for friend, newish members, FUD, are RED FLAGS. A video conference call is not adequate assurance. Face to face interactions are required. Please report suspicions to the forum admins. Stay Safe - anyone can get scammed.

Chamfering tool bits

jcdammeyer

jcdammeyer

John
Premium Member
With all the robot arm parts I'm milling out I normally just use my manual edge deburring tool like this one from PA.

But programming the CNC to follow the edge and do it automatically is much nicer. What angle tool is used for this?
From AliExpress there are all sorts.
www.aliexpress.com

HRC58 Chamfer Milling Cutter 30 40 45 50 60 70 80 90 100 110 120 130 140 150 Degree Carbide Corner Countersink Chamfering Mill - AliExpress 1420

Smarter Shopping, Better Living! Aliexpress.com
www.aliexpress.com www.aliexpress.com
Wouldn't one just use a 90 degree tool to create a 45 degree edge? Or are there reasons to use a 30 degree or 45 degree tool bit?
 
That is entirely your call. For general purpose work, looks good - go with the 45 chamfer (90 degree included angle on the tool). I have a few jobs that call for other angles, not a big deal, it is just a different tool (same process of calling the perimeter path). Generally there would be a reason if one were to go other than 45 (the edge has to mate up against another surface, maybe there is a seal).
 
ChazzC said:
Perfect for router bits.
Click to expand...
I'd though of that but there are smaller cut-outs that require something more like a 6mm diameter bit. However, as @DavidR8 saw yesterday, the 0.025" backlash in the X Axis ACME screw causes all sorts of issues and so I've not pressed the idea of chamfering concept.
Yet...
 
John,

There are a LOT of great carbide milling tools out there that will get you what you need, in sizes from "need a forklift" to "Need a Microscope to see".

Per your question as to why one set of degrees over another, it usually revolves around what the print calls out!

Classic example of the least used Mil-Spec! MIL-TFD-41-A! Aka, Make It Like the F***ing Drawing For Once A-Hole! :)

I have seen catalog listings of angles ranging from a single degree of taper to an included angle a bit sort of 180 degrees, and have custom ordered bits of the diameter I wished, with anything from a stated angle and width, at the corners, to both inside and outside radii.

M A Ford was good to me in the past. Pretty sure about any genuine Supplier can get you about anything you might want, if you can wait for a Custom Order (which, in my experience, was NOT a long wait!). Prices were not out of line for the stocked tools either.
 
trevj said:
John,

There are a LOT of great carbide milling tools out there that will get you what you need, in sizes from "need a forklift" to "Need a Microscope to see".

Per your question as to why one set of degrees over another, it usually revolves around what the print calls out!

Classic example of the least used Mil-Spec! MIL-TFD-41-A! Aka, Make It Like the F***ing Drawing For Once A-Hole! :)

I have seen catalog listings of angles ranging from a single degree of taper to an included angle a bit sort of 180 degrees, and have custom ordered bits of the diameter I wished, with anything from a stated angle and width, at the corners, to both inside and outside radii.

M A Ford was good to me in the past. Pretty sure about any genuine Supplier can get you about anything you might want, if you can wait for a Custom Order (which, in my experience, was NOT a long wait!). Prices were not out of line for the stocked tools either.
Click to expand...
I have both 90 and 60 degree bits. What I'm not sure about is how to program the CAM to create that bevel around the outside.
Granted I haven't done any research on how to do this but as I understand it you just get the center line of the tool bit to follow the profile? Then depending on the Z position the bevel can be small or large?
 
jcdammeyer said:
I have both 90 and 60 degree bits. What I'm not sure about is how to program the CAM to create that bevel around the outside.
Granted I haven't done any research on how to do this but as I understand it you just get the center line of the tool bit to follow the profile? Then depending on the Z position the bevel can be small or large?
Click to expand...
Yes, but... there is a tool standoff as well - i.e. the shank must stay clear of the end of the edge because it would run into a wall. The chamfer toolpath will have a setting for that, the value is usually 1/2 the tool diameter, but if you are using the upper part of the flutes, the shank clearance can be very small.
IMG_5134.JPG
 
jcdammeyer said:
I have both 90 and 60 degree bits. What I'm not sure about is how to program the CAM to create that bevel around the outside.
Granted I haven't done any research on how to do this but as I understand it you just get the center line of the tool bit to follow the profile? Then depending on the Z position the bevel can be small or large?
Click to expand...
I’m sure there are a few ways to approach this, the suggestions above are all good. I do a lot of chamfer work with the CNC mill (it really sets off a component nicely). I don’t use any CAM program at all (yet another thing I need to learn). My approach (probably a pretty common technique) is to program the tool bit center line - straight line, curve etc. - line by line G1 & G2/G3 (or holes or pins a G175/176), whatever, sort of like one would with a manual machine but send a line of code. The trick here is to invoke CDC (cutter diameter compensation) for those moves. Obviously the ramp in is done off part in a safe location. A cool aspect is that you can adjust the amount of chamfer by the depth of the tool or by how much CDC you call out - and it affects the whole tool path. Once you have it sorted out (which side to compensate (G41/G42) and how it ramps on/off you’ll use it often.
 
ChazzC said:
You didn’t say what material you’re using, but for Aluminum I’ve switched to 1/2” shank Carbide router bits: make beautiful rounded edges.
Click to expand...
I use 'em on steel. They work well, leave a nice finish and, best of all, they're cheap!
www.ebay.com

6X 1/2" Shank Round Over Router Bits R1/8-R1/2 Corner Forming Beading Router Bit | eBay

Specification: Type: Coner Round Over Edging Router Bit Material: Tungsten Carbide Shank: 1/2''(12.7mm) Radius: R1/8''(3.175mm) R3/16''(4.76mm) R1/4''(6.35mm) R3/8''(9.5mm) R5/16''(7.96mm) R1/2''(12.7mm) Package Including: 6pcs Corner Round Over Router Bits.
www.ebay.com

 
Got it! Here's the simulation.
1731517585324.png

With these parameters

1731517658634.png


And I can define the tool here as a V Mill. The software is smart enough to know if the tool holder will run into a wall based on tool length and holder size. I set the max dimensions of the TT collet holder.
1731517731113.png
 
DavidR8 said:
What CAM is that John?
Click to expand...
Well it was AlibreCAM (still is although it crashes regularly with an invalid pointer error) but it's actually MECSOFT VISUALCAM which is part of their advanced VISUALCAD/CAM software offering.

The demo software lets you do the same thing with the .STEP file that it can import but of course I can't save it.

mecsoft.com

VisualCAD/CAM: Standalone CAD/CAM Software for CNC machining | Try for Free | MecSoft Corporation

VisualCAM/CAD is our standalone CAD/CAM package that is the best valued software on the market today. Try our Free Demo Today!
mecsoft.com mecsoft.com

1731518603212.png
 
I mostly use a 4mm 90-degree 3-flute carbide to chamfer. Something like https://www.amazon.ca/dp/B095LSGC4T Obviously something larger on large parts!

For CAM, make a toolpath that is 0.05 from the edge (outward for outside and inward for holes). Run the bit on the created toolpath. Typically I plunge the chamfer tool to 0.035 below the top surface and cut to 0.07 below the top surface. 10000 rpm and 20ipm.

You can see the results on the heatsink that I sent to you last week.
 
kstrauss said:
I mostly use a 4mm 90-degree 3-flute carbide to chamfer. Something like https://www.amazon.ca/dp/B095LSGC4T Obviously something larger on large parts!

For CAM, make a toolpath that is 0.05 from the edge (outward for outside and inward for holes). Run the bit on the created toolpath. Typically I plunge the chamfer tool to 0.035 below the top surface and cut to 0.07 below the top surface. 10000 rpm and 20ipm.

You can see the results on the heatsink that I sent to you last week.
Click to expand...
Yes. It looked good. IIRC, you're using a TORMACH right? Is that with their latest user interface on top of LinuxCNC? I've read it's possible to install that on other hardware but would take some effort. At the moment I still am having problems with my tool height measure and install into tool table. Decided I needed a holiday from that for a week or so as I was getting way too frustrated.
 
DavidR8 said:
You don't ever use a CAM program? How do you make complex shapes?
Click to expand...
You are correct, it is a problem. I don’t do any 3D surface profiling. I have not done any letter engraving. I think your point is that I am limiting myself. You would be right in that. My machine is a DX32 dialect (still G code, but it’s own peculiarities) - so if you know a competent DX32 post processor, please share. Fusion will sort of do DX32, I worked through Titan’s first mill project tutorial - the resulting file was too big to load. The resident memory is only a few hundred kB, which is plenty when you are writing the code, but gets eaten up quickly with computer generated code (lots of little moves where I would have used a small number of more capable instructions) - big programs can be drip fed (again something else to figure out).

Also what is a “complex shape”? Please define it. One can do a lot with a collection of simple shapes, the end result might look complicated, but it is just a bunch of simple shapes put together (straight lines, circular lines, helical lines in about any plane). For example jaws for a 3J chuck, the curved teeth appear complicated. That shape is just a spiral path (G12/13 helical interpolation) - on my machine each tooth is just two lines of code, followed by the appropriate offset, repeated several times.

I have made a lot of different parts, the only thing I have avoided is letter engraving. The direct coding works well enough that there is little motivation to sort out a CAM program (granted it is on that “some day” list). I am usually doing fairly small programs, not a large number of parts, to me it is a significant benefit to be able to tweak / edit the program at the machine - depending on the edit, it might just be a few seconds. A “big” program is perhaps 100 lines, pretty easy to find the edit location.
 
Chipper5783 said:
You are correct, it is a problem. I don’t do any 3D surface profiling. I have not done any letter engraving. I think your point is that I am limiting myself. You would be right in that. My machine is a DX32 dialect (still G code, but it’s own peculiarities) - so if you know a competent DX32 post processor, please share. Fusion will sort of do DX32, I worked through Titan’s first mill project tutorial - the resulting file was too big to load. The resident memory is only a few hundred kB, which is plenty when you are writing the code, but gets eaten up quickly with computer generated code (lots of little moves where I would have used a small number of more capable instructions) - big programs can be drip fed (again something else to figure out).

Also what is a “complex shape”? Please define it. One can do a lot with a collection of simple shapes, the end result might look complicated, but it is just a bunch of simple shapes put together (straight lines, circular lines, helical lines in about any plane). For example jaws for a 3J chuck, the curved teeth appear complicated. That shape is just a spiral path (G12/13 helical interpolation) - on my machine each tooth is just two lines of code, followed by the appropriate offset, repeated several times.

I have made a lot of different parts, the only thing I have avoided is letter engraving. The direct coding works well enough that there is little motivation to sort out a CAM program (granted it is on that “some day” list). I am usually doing fairly small programs, not a large number of parts, to me it is a significant benefit to be able to tweak / edit the program at the machine - depending on the edit, it might just be a few seconds. A “big” program is perhaps 100 lines, pretty easy to find the edit location.
Click to expand...
That's fascinating. For full disclosure I am a CAM newbie (kindergarten level) so the idea of writing the G-code for something other than a straight line move is beyond me.
I'd be very interested in seeing an example of a 2D shape you've milled and its corresponding G-code.
 
You must log in or register to reply here.
Back
Top