Segmented rounds

[Antoine21130]

Adding something to this about accuracy or precision numbers in Fusion (or any CAM for that matter): those only apply when it's doing conversion of non-arc curves (splines, ellipses) or surfaces into line moves. If your output is G02/G03 moves, accuracy doesn't weigh into the problem.

Arc moves are strictly up to the control to execute them right or wrong. If anything, you should be checking the Yasnac control if it has its own tolerance / accuracy setting for how fine it breaks up circular moves.

As already posted: speed might be a factor. The extremely small amount of clearance between rough and finish cuts probably plays into it. If you're jamming a cutter down there and doing full-depth cuts, that also plays into it. I'd personally do a helical cut around each of those posts and not treat them like pockets.

The artifacts left on the chamfers look like the cutter needs a rough and finish lap around the part. It's probably deflecting at the end and not completing the circle.

Ok that confirms what I was thinking about tolerances (tried changing them and not that much of a difference in the code).

I will try to reduce my speeds as triumph also advised me to do.

Your idea of doing helical cut around each boss also seems better than doing a pocket.

Thanks a lot for all theses advices !

 

[Houdini]

Adding something to this about accuracy or precision numbers in Fusion (or any CAM for that matter): those only apply when it's doing conversion of non-arc curves (splines, ellipses) or surfaces into line moves. If your output is G02/G03 moves, accuracy doesn't weigh into the problem.

Arc moves are strictly up to the control to execute them right or wrong. If anything, you should be checking the Yasnac control if it has its own tolerance / accuracy setting for how fine it breaks up circular moves.

Yup 100%

As already posted: speed might be a factor. The extremely small amount of clearance between rough and finish cuts probably plays into it. If you're jamming a cutter down there and doing full-depth cuts, that also plays into it. I'd personally do a helical cut around each of those posts and not treat them like pockets.

The artifacts left on the chamfers look like the cutter needs a rough and finish lap around the part. It's probably deflecting at the end and not completing the circle.

actually the chamfers look to me like he has a tool vs geometry issue, looks like its programmed incorrectly, and we are seeing the entry and exit of the path.

 

[Antoine21130]

Yeah I think chamfer is really related to how I programmed it because each artifact is located exactly at each in/out of the path. I’ve found the setting to make few more millimeters to fully chamfer.

 

[Donkey Hotey]

actually the chamfers look to me like he has a tool vs geometry issue, looks like its programmed incorrectly, and we are seeing the entry and exit of the path.

I was thinking the same thing but, I can't figure out how a conical cutter would leave that shape if it started and stopped at the same point on the circle. I totally agree that I've seen those artifacts left on open segments but, not a closed one. Then again, I don't know what the in-out moves look like. Mastercam has an option to extend the start and ends of elements that would clean that up. Not sure in Fusion.

 

[Houdini]

I was thinking the same thing but, I can't figure out how a conical cutter would leave that shape if it started and stopped at the same point on the circle. I totally agree that I've seen those artifacts left on open segments but, not a closed one. Then again, I don't know what the in-out moves look like. Mastercam has an option to extend the start and ends of elements that would clean that up. Not sure in Fusion.

I know what you mean, it looks almost like a cutter comp vs programming error. Like its comping it away form the same point as we would normally see, leaving a radial gap at the in/out

 

[DavidScott]

Adaptive roughing does not leave smooth sidewalls, or posts, which is what I see as one of the problems. I doubt leaving .002" a side in that roughing routine will be enough. The chamfers look like they are relatively smooth except for the enty/exit point, try more of an overlap or path extension to clean that up.

 

[Houdini]

Adaptive roughing does not leave smooth sidewalls, or posts, which is what I see as one of the problems. I doubt leaving .002" a side in that roughing routine will be enough. The chamfers look like they are relatively smooth except for the enty/exit point, try more of an overlap or path extension to clean that up.

adaptive roughing is what I said, the floor matches the walls in the image, adaptive usually has a large default tolerance setting for speed also, if not enough left to clean it gouges fo sho!
a .010" roughing tolerance with a .002" wall cleanup = OUCH!

 

[Nerdlinger]

Yeah I think chamfer is really related to how I programmed it because each artifact is located exactly at each in/out of the path. I’ve found the setting to make few more millimeters to fully chamfer.

The chamfer totally looks like it is just incomplete...in my ancient version of MasterCAM there is an "overlap" checkbox I often use whereby if the circle starts at 12 o'clock and goes clockwise instead of exiting right at 12 o'clock again it will exit at, say, 1 o'clock. It kind of looks like your entries are starting and exits are ending at the same point, meaning the moves are starting a bit early...before all 360 degrees of chamfer have been completed.

ALSO, something I think I see that you may not know but hopefully will help - it looks like the cutter is digging in a bit more on the left side of those entry/exit marks. That happens often upon exits as the cutter approaches the area where there is less material in front of it so tool deflection straightens out and thusly takes off more material. I hope that makes sense. Good luck!

 

[Antoine21130]

600mm/min is too fast. especially as your running around a 3mm round. Your feedrate at the circumference of the 3mm round is too high.

I typically program .0002-.0003ipt and use 3 flute YG-1 endmills

10000*3*.0003 = 9in/min

but going around those features I would start at 2-3in/min and do 2 finish passes

I assume your running the chamfer tool way to fast as well

How do you define that .0002/.0003ipt value ? I don’t have a lot of experience with these values so I used manufacturer data sheet (dormer) that gives a value of 0.025mm/tooth for my 3mm 4flutes endmill (DOC is 1.7mm in my case and I limited the WOC to 0.3mm).
What I understand is that I have to greatly reduce values given by the manufacturer ?

 

[Antoine21130]

The chamfer totally looks like it is just incomplete...in my ancient version of MasterCAM there is an "overlap" checkbox I often use whereby if the circle starts at 12 o'clock and goes clockwise instead of exiting right at 12 o'clock again it will exit at, say, 1 o'clock. It kind of looks like your entries are starting and exits are ending at the same point, meaning the moves are starting a bit early...before all 360 degrees of chamfer have been completed.

ALSO, something I think I see that you may not know but hopefully will help - it looks like the cutter is digging in a bit more on the left side of those entry/exit marks. That happens often upon exits as the cutter approaches the area where there is less material in front of it so tool deflection straightens out and thusly takes off more material. I hope that makes sense. Good luck!

Yeah worked on the chamfering today and it was just incomplete (added overlap in fusion and that fixed it).

Thanks for the explanation/analysis on the tool deflection ! Any knowledge is appreciable haha.

 

[Antoine21130]

Adaptive roughing does not leave smooth sidewalls, or posts, which is what I see as one of the problems. I doubt leaving .002" a side in that roughing routine will be enough. The chamfers look like they are relatively smooth except for the enty/exit point, try more of an overlap or path extension to clean that up.

Yeah wasn’t aware of that, also tried 2D pocketing but as it’s also a roughing strategy I got quite the same result

 

[DavidScott]

600mm/min is too fast. especially as your running around a 3mm round. Your feedrate at the circumference of the 3mm round is too high.

I typically program .0002-.0003ipt and use 3 flute YG-1 endmills

10000*3*.0003 = 9in/min

but going around those features I would start at 2-3in/min and do 2 finish passes

I assume your running the chamfer tool way to fast as well

He is on a Matsuura, not a Fadal. For a 1/8" stub 3 flute mill for aluminum I would be running .002" ipt as a general starting point.

This brings up another question, what end mill are you using? You say 4 flutes so that is not something we would use in aluminum for this type work.

 

[Antoine21130]

I’m using a dormer 4 flutes MCX 904 3mm and the docs said it was « good for ramping/slotting applications in aluminium » so tough it was ok. Less flutes is better for chip evacuation right ?

 

[triumph406]

How do you define that .0002/.0003ipt value ? I don’t have a lot of experience with these values so I used manufacturer data sheet (dormer) that gives a value of 0.025mm/tooth for my 3mm 4flutes endmill (DOC is 1.7mm in my case and I limited the WOC to 0.3mm).
What I understand is that I have to greatly reduce values given by the manufacturer ?

The manufacturers data is only a starting point.

You have an issue, therefore you have to try different settings to get a good result. .025mm/tooth is .001ipt, I would consider that too be too fast at face value. imho

And certainly I would be running spring passes as a matter of policy. ymmv

I think the .0002-.0003 might have come from FSWizard an Iphone app.

 

[triumph406]

He is on a Matsuura, not a Fadal. For a 1/8" stub 3 flute mill for aluminum I would be running .002" ipt as a general starting point.

If I got that finish on one of my Fadals the OP is getting I'd take it out and shot it.

 

[Antoine21130]

Ok thanks ! Just wanted to know why these values where so different. Of course I will try different settings and going slower can only help with my issue (at least I think so).

 

[???]

You should change your post heading to facetting on OD or similar. When you said segmented rounds I thought you meant the sabot that goes around a APFSDS tank round .

 

[triumph406]

Ok thanks ! Just wanted to know why these values where so different. Of course I will try different settings and going slower can only help with my issue (at least I think so).

I rarely run production, mostly proto/r&d work. So I'm not bothering to try and optimise every tool path,every feedrate, every tool type etc etc I go with what works for me, which is being conservative. I prefer reliability based on what I know works for me rather then pushing the boundaries.

 

[Antoine21130]

Hello everyone, finally managed to get a good boss geometry ! Changed to a 2.5mm mill, reduced my speeds and left more material before the finishing pass.
Thanks a lot for all the help.

 

[Antoine21130]

You should change your post heading to facetting on OD or similar. When you said segmented rounds I thought you meant the sabot that goes around a APFSDS tank round .

Haha yeah sorry. How do you change post heading ? Can find how to do that.