What's new
What's new

Wall finish with dormer S903

Antoine21130

Aluminum
Joined
Oct 19, 2023
Hello everyone,

I’m having a hard time getting a good wall finish with a 3mm dormer S903 3 flutes carbide endmill on my Matsuura MC-660.

Recommend feed per tooth is 0.019mm/rev and recommended surface speed is 179 M/min.

Spindle is limited to 15000/min so I used a 120 m/min surface speed.

I tried lower feed/tooth, higher feed/tooth, slower surface speed but can’t get a good finish as you will see in attached pics.

I’ve left 0.1mm before finishing pass and also tried 0.2mm.

I’ve also checked runout which is approx 0.01mm. (You will see holder type in attached pics)

I get a mirror finish with a cheap 6mm Chinese endmill without issue so I think I should be able to get the same or better with the dormer but can’t even get something acceptable.

I don’t really know where to look next so that’s why I’m asking for your help and knowledge !

Thanks in advance :)
 

Attachments

  • IMG_9315.jpeg
    IMG_9315.jpeg
    1.4 MB · Views: 34
  • IMG_9310.jpeg
    IMG_9310.jpeg
    1.7 MB · Views: 33
  • IMG_9312.jpeg
    IMG_9312.jpeg
    2 MB · Views: 33
It looks like that tool holder has been through a couple wars. How much runout do you have at the end of your endmill?

Also, is Dormer a high quality brand? I've never heard of them. And this endmill is half the size of your chinese endmill, so of course you'll be fighting a different fight.
 
0.1mm WOC and 3mm DOC I also tried with a 2deg ramp and 2mm max DOC with quite the same result. Also tried 0.2mm WOC
 
It looks like that tool holder has been through a couple wars. How much runout do you have at the end of your endmill?

Also, is Dormer a high quality brand? I've never heard of them. And this endmill is half the size of your chinese endmill, so of course you'll be fighting a different fight.
Yeah holder is not new haha but runout at end of endmill is 0.01mm. And yeah dormer is a high quality brand.
 
The runout isn't helping you any.

Also, have you actually verified that you're taking .1mm (.004") WOC? In other words, is your rougher leaving what you think it's leaving?

I've occasionally had a new endmill be 'too sharp' and chatter when I know it shouldn't. I don't know exactly what the cause is, but running a stone VERY LIGHTLY down the cutting edge of each flute will dull it enough to kill the chatter. I can't say this will solve your problem, but it's an option.

As a test, you can try cutting your RPM in half and keeping the same chip load to see what that does.
 
The runout isn't helping you any.

Also, have you actually verified that you're taking .1mm (.004") WOC? In other words, is your rougher leaving what you think it's leaving?

I've occasionally had a new endmill be 'too sharp' and chatter when I know it shouldn't. I don't know exactly what the cause is, but running a stone VERY LIGHTLY down the cutting edge of each flute will dull it enough to kill the chatter. I can't say this will solve your problem, but it's an option.

As a test, you can try cutting your RPM in half and keeping the same chip load to see what that does.
So I should try to reduce the runout ? What kind of values are acceptable for runout on such small tool ?

Yes I verified the walls after roughing and finishing op is really taking 0.1mm.

Endmill is really sharp like a razor so maybe I can try that.
 
You're cutting the outside of that block. What made you decide on that tiny end mill?
Use a larger one and be done with it.
This block is just a test piece to show the issue. I’m getting this issue on every feature where I need to use that endmill so just made few test cuts on a simple square to adjust my cutting condition and find the cause of that issue.
 
Well looking at you params (fkn metric!)
Looks like your runout is too high need to get it down to .0001" , .0002" max.

and from the image the tool is sticking out 6XD so the RPM for that noodle cutter is too high.

and I have not been impressed by and Dormer tooling. i have some expensive index mills and they suck.
 
Your speeds, feeds and W.O.C. all seem fine, like Matt said, lightly stone the cutting edges and see if that helps.

One thing I would check is to see if your retention knob is loose on that holder.
 
Well looking at you params (fkn metric!)
Looks like your runout is too high need to get it down to .0001" , .0002" max.

and from the image the tool is sticking out 6XD so the RPM for that noodle cutter is too high.

and I have not been impressed by and Dormer tooling. i have some expensive index mills and they suck.
Haha sorry for the metric value, will convert them next time. I will adjust runout as best as I can and try again.

I’ve used dormer on other sizes (6 and 8mm) and got quite decent results and tool life but I’ve not tested many other brands so I can’t really compare these results
 
Your speeds, feeds and W.O.C. all seem fine, like Matt said, lightly stone the cutting edges and see if that helps.

One thing I would check is to see if your retention knob is loose on that holder.
I checked the pull stud and it’s not loose. I will also try to stone the cutting edges as you recommended and change tool holder to see if I get any difference. I don’t really think it’s tool deflection cause I also tried some really small WOC and get the exact same results.
 
Yeah you have to take the context of the small size into the factors.
at .0004" runout on a tool that is only .118", and then it is hanging out 6XD, and spinning at 15,000rpm.

yeah without even trying you know it isn't going to work.
 
Yeah you have to take the context of the small size into the factors.
at .0004" runout on a tool that is only .118", and then it is hanging out 6XD, and spinning at 15,000rpm.

yeah without even trying you know it isn't going to work.
Thanks for that synthesis haha, only started recently so don’t have all necessary knowledge to know and “feel” if parameters are optimal or not. (I’m running at 12700 rpm but I think it’s quite the same as 15000 rpm in your analysis)
 
Thanks for that synthesis haha, only started recently so don’t have all necessary knowledge to know and “feel” if parameters are optimal or not. (I’m running at 12700 rpm but I think it’s quite the same as 15000 rpm in your analysis)
Yeah the 6XD and .0004" runout is killing you.
Could be worse, I have ran some .062" at over 30XD, good times. :D
 
So I changed the tool holder and tried to adjust the runout.
Problem is that i get a runout of approx 0.0001" on two of the flutes but 3rd flute shows a much higher runout of approx 0.0005" (measured using an indicator and counterclockwise rotation of the toolholder).

Should I blame the endmill ? I can't understand how the runout can only show on one of the flutes.
 
Put a solid carbide shank in your holder and check the runout on that. You're only checking runout at 3 small points along a circle.

That endmill is sticking out 5 or 6 diameters long. They are more likely to chatter at that ratio.

A few things to help:

lower runout (obviously)

less stickout

if you need that amount of stickout, slower rpm may help. Also, higher feed may also help.

If you need to get deeper with such a small endmill, you could try an endmill with necked shank and less flute length, do it in several passes.

Any type of variable flute / variable helix may help with chatter.

You probably don't need a 3 flute if you are only using it for finishing .1mm on the walls. 3 flute is better when hogging or slotting and you need room for chips to evacuate.
 
Yeah your runout is horrible.
Start at the top and work your way down.

put a solid tool, or a collet holder tool in with no collet or nut, and check the tool holder runout in the spindle.
try a couple if its bad.

check spindle taper for chips or bumps.

then you can start checking tool holders.

as mentioned, but you can put a long tool in and check higher up on the shank of the tool, not on the flutes.
of if you have a solid piece of carbide, a long tool loaded in backwards, but the flutes cannot touch the collet, must go in deep.
 








 
Back
Top