What's new
What's new

Chamfer overshoot on arcs

Antoine21130

Aluminum
Joined
Oct 19, 2023
Hello everyone,

Another newbie question !

I’m having a hard time understanding why my chamfers are larger that programmed only on arcs geometry. I’m using a 12mm 90 deg 3 flutes chamfer tool on aluminium.

You can see the issue on rounded parts of hexagonal pockets :72798788703__0FF18AB2-B58B-4283-9C3A-3F529F8D038B.jpeg

I’ve searched on the net without success after struggling with understanding how that can happen. It seems to me like it’s a kind of « overshoot » or tolerance issue but maybe I’m completely wrong.
 
Good chance your chamfers are correct and the pockets are undersize in the corners. Have you measured them?
Yes, this. Either your pocketing endmill is too big (unlikely but a possible beginner mistake), or your control is "cheating the corner" so it doesn't violate the wall geometry. If you are not running some sort of high-accuracy parameter, and if your chamfer tool is running much slower than your pocketing EM, this is what happens.

What machine?
What speed and feed for the pocketing endmill and the chamfer tool?

Regards.

Mike
 
will have to check tomorrow for the size of pockets. Endmill for pocketing is a 4mm 3 flutes and internal corner radius is 2mm (maybe not the best choice to force the endmill like that ?)

Pocketing endmill is running at 1260mm/min and 12000 rpm and chamfer tool is at 480mm/min and 4000 rpm (tried a low speed to see if that helped).

I’m not running any kind of high accuracy parameters.

Machine is Matsuura MC-660-VG with 15k rpm spindle and Yasnac J-300M.
 
What's the tip depth offset on the chamfer mill ?. 12mm chamfer tool, 2mm pocket corner ?, overcutting ?. Should show in simulation if using CAM.
 
0.8mm tip depth offset (not a lot of room with the bottom of the pocket). Everything in the simulation from fusion looks good so I don’t think that’s over cutting.

Don’t know if it can be related but I also have a place where chamfer is not done if I don’t set a path extension of approx 1mm. It seems like the chamfer tool is starting to move in x and y just before reaching the correct Z depth. I don’t see it in simulation, only when machining.

Another thing to note, when making chamfer on smaller geometry with same parameters (to edge of a 3mm slot for example) I hardly have any chamfer but in simulation I get exactly the same chamfer as on a larger geometry.
 
If the pockets are programmed with sharp corners the tip of the chamfer cutter could be a smaller diameter than the 4mm end mill. If this is the case the chamfer cutter toolpath needs to have a 2mm corner radius.
 
Show us a CAD/CAM screenshot, with dimensions if possible.

Win+shift+s to get a screengrab -> copy -> paste into your reply and resize as necessary
 
If the pockets are programmed with sharp corners the tip of the chamfer cutter could be a smaller diameter than the 4mm end mill. If this is the case the chamfer cutter toolpath needs to have a 2mm corner radius.
I think fusion is doing the right thing. I have sharp corners when pocketing and 2mm radius on the chamfer tool path.
 
Here are the dimensions of the hexagonal pocket :

hexagon.png

And correction, feed for the 4mm endmill for contouring was 2230 mm/min (was tired last night haha).

Here is the toolpaths for contouring and chamfering :

contouring.png chamfer.png
 
Your endmill finish pass is at 2230mm/min (thats about 80 inches a minute)?

Can't tell very well from the pictures but your corner radii don't look as small as your cad illustration. Many machines, when telling them to go fast, will round corners. On pockets, fast feedrates will leave a much larger radius than programmed because the machine has to start changing direction earlier.

So, try to slow it down first, see if it makes a difference.

Edit: by slow, I mean start with something like 700mm/min to start. Those are not very large pockets.

Edit2: Finegrain and gregormarwick were on to this idea above.
 
Your endmill finish pass is at 2230mm/min (thats about 80 inches a minute)?

Can't tell very well from the pictures but your corner radii don't look as small as your cad illustration. Many machines, when telling them to go fast, will round corners. On pockets, fast feedrates will leave a much larger radius than programmed because the machine has to start changing direction earlier.

So, try to slow it down first, see if it makes a difference.

Edit: by slow, I mean start with something like 700mm/min to start. Those are not very large pockets.

Edit2: Finegrain and gregormarwick were on to this idea above.
Yes about 87 inch/min. And it seems like Finegrain and Gregormarwick are right, endmills is taking a path with a larger radius. I will try to slow down and I think it should improve.

I also have HON HOFF on control so maybe that can help with that behavior ? G64/G61 can also help with that kind of issue right ?
 
Yes about 87 inch/min. And it seems like Finegrain and Gregormarwick are right, endmills is taking a path with a larger radius. I will try to slow down and I think it should improve.

I also have HON HOFF on control so maybe that can help with that behavior ? G64/G61 can also help with that kind of issue right ?

I don't know what HON HOFF means at least in this context. G61 is exact stop, it might improve the corner rounding slightly, but only insofar as it will force the control to slow down a bit. It's not what it's for. If you use G61 on your example, the tool will decelerate to a stop on the straight side of the pocket, then will accelerate as fast as it can round the corner.

Modern controls have functions to dynamically adjust feed and acceleration to prevent this, and some controls do it by default, even some really old ones. I have never touched a Yasnac, so I don't know what functions you have at your disposal.

If none for this purpose, most decent cam software will have ways to mitigate it, by posting reduced feedrates for internal arcs etc.
 
HON enable high speed machining on the J300.

I also have G107-G108 for corner speed reduction in the Yasnac J300 so I think that’s that you refer to.

And yes fusion can post reduced feedrate for internal arcs.

Thanks for the explanation on G61 !
 
And yes fusion can post reduced feedrate for internal arcs.

But I don't think you have any internal arcs. Your drawn radius is the same as the tool radius.

If you drew the radius as 2.1mm you might be able to achieve it with slowed arc feedrate, but not like you currently have it.

Alternatively you could profile it with a 3mm tool.


Also, I think I would start even slower, maybe 500mm/min to start. Unless you do actually make radius movements in the corners, instead of simple G1 direction changes.
 
But I don't think you have any internal arcs. Your drawn radius is the same as the tool radius.

If you drew the radius as 2.1mm you might be able to achieve it with slowed arc feedrate, but not like you currently have it.

Alternatively you could profile it with a 3mm tool.


Also, I think I would start even slower, maybe 500mm/min to start. Unless you do actually make radius movements in the corners, instead of simple G1 direction changes.

I missed that. In that case, yes G61 will fix it, but the tradeoff is likely to be an unsatisfactory finish in the corner.

It's never good practice to use the full tool radius in a corner.
 
But I don't think you have any internal arcs. Your drawn radius is the same as the tool radius.

If you drew the radius as 2.1mm you might be able to achieve it with slowed arc feedrate, but not like you currently have it.

Alternatively you could profile it with a 3mm tool.


Also, I think I would start even slower, maybe 500mm/min to start. Unless you do actually make radius movements in the corners, instead of simple G1 direction changes.
I think fusion can also slow done if an angle is higher than a given angle. But yes you’re right, my tool path doesn’t contain an arc.

And yes I will use a smaller tool for that task and reduce my feed.

Thanks a lot for your help. Will come back to give the results after reducing the feed.
 
You have HON option?
If yes turn it on
Also finish with smaller tool.
I can send you my post for yasnac/matsuura. some stuff like pallet change would be no use for you, but other thing should be right ap your alley
 
Yes I have Hon option but haven’t tried it for now.

Oh yes i would really appreciate it because for now I’m running with the default Yasnac post !
 








 
Back
Top