[jmvar]

I know this is a very general question and I will post more details about my specific situation as soon as I have access to my personal computer.

I am using a PC1100 with a Maritool 1/4" carbide 3 flute finishing endmill with flutes 1.25" in length on 6061. I am trying to take a .962" DOC cut and I am optimizing it using Gwizard to ensure I am running the correct feeds and speeds. So far if I use the finish setting on Gwizard I am getting a lot of chatter squeeling from the endmill and a poor surface finish. Set up is a TTS ER20 tool holder with a collet supplied by tormach. The stock is clamped tight in the vise and seems rigid enough. Using a fog buster with coolant.

Things I plan on trying:
- measure runout and try using a rego-fix high precision collet
- try different feeds and speeds from Gwizard

My basic question is has anyone successfully run a .25" endmill this long in a PC1100? I want to try and resolve my issue but I am wondering if the PC1100 is just not rigid enough to run an endmill this long and this thin?

Any insights and suggestions are greatly appreciated. I will post up more details on my setup tonight with pics of the finish I am getting.

[SCzEngrgGroup]

I would be amazed if you could get that DOC with a tool that long without chatter. I would not go beyond probably 0.250" DOC, if that.

Regards,
Ray L.

[jmvar]

I would be amazed if you could get that DOC with a tool that long without chatter. I would not go beyond probably 0.250" DOC, if that.

Regards,
Ray L.

Hi Ray, thanks for the response. Is this a factor of the PC1100 not being rigid enough or the width to length ratio of the cutter? I appreciate the response as this is all pretty new to me.

[SCzEngrgGroup]

Hi Ray, thanks for the response. Is this a factor of the PC1100 not being rigid enough or the width to length ratio of the cutter? I appreciate the response as this is all pretty new to me.

No, just the length of the tool. A 1/4" 3-flute tool that long will be like a piece of cooked spaghetti. You'll either have to take extremely light radial cuts, or much smaller vertical steps.

What radial depth, RPM and feed were you using?

Regards,
Ray L.

[jmvar]

No, just the length of the tool. A 1/4" 3-flute tool that long will be like a piece of cooked spaghetti. You'll either have to take extremely light radial cuts, or much smaller vertical steps.

What radial depth, RPM and feed were you using?

Regards,
Ray L.

I took a finish pass at DOC: .962" WOC: .0015" F: 43 ipm S: 5100 rpm as suggested by Gwizard.

Thanks

[pickled]

You MAY be able to get 2 x DOC with that tool. Pushing it to and/or beyond .5" is definitely a recipe for chatter with a 1/4" carbide tool. Try to break the cut up into 2 passes and then optimize depth of cut from there.

[SCzEngrgGroup]

I took a finish pass at DOC: .962" WOC: .0015" F: 43 ipm S: 5100 rpm as suggested by Gwizard.

Thanks

HSMAdvisor, which I trust FAR more than G-Wizard, gives that same RPM and feed for only a 0.5" depth... It won't even allow me enter 0.962" depth, which means it's not a realistic cut. IME, HSMAdvisor is almost always right, and if it's not, the fault usually lies in either the machine or the tool.

Regards,
Ray L.

[Hirudin]

A few suggestions (I'll number them to make them easier to ridicule )

1. Do you know the helix angle of the bit you're using? A higher helix angle may reduce chatter. I accidentally recorded a video where I ended up comparing some tools with different helix angles. The tools also had different coatings and were from different manufacturers, which I realize makes for a poor test, but when I started I was just intending to record the performance of a single bit. Only after it started squealing like stuck pig did I end up changing to other bits. And it wasn't until I was done with the part and started editing the video that I realized the helix angle was probably the most important change.
I guess I should actually link to the video...
https://www.youtube.com/watch?v=CyNkCqthtog

2. I'm going to guess you're doing climb milling. You might consider conventional milling as apparently the angle of deflection varies between climb and conventional milling. That's what this CNC Cookbook article says anyway: Climb Milling vs Conventional Milling
(Look for the Tool Deflection and Cut Accuracy in Climb vs Conventional Milling section if you want to skip straight to the part I'm referring to.

3. You may actually get better results if you increase the WOC. With only 1.5 thousandths to bite on, your cutter might be making some super tiny/thin chips, which aren't ideal. I'd definitely recommend bumping this up if you switch to conventional milling (~10 thousandths (0.010") or so is prolly good).

4. Check out the feeds and speeds recommended by the nifty calculator CNCZone member Bryan Turner made. I plugged in your numbers (I think I got them all) and hit the button to turn the inputs into this link right here
Hopefully that works. I bumped the deflection down to 0.0001". Click the "Compute" button a few times to get more results.

[Steve Seebold]

At 5100 RPM and 43 IPM you're running it WAAAAAYYYYY too fast.

What are you doing with that cutter/ Are you ruffing or just finishing?

For a .962 depth of cut with a 1/4 inch end mill I wouldn't try to take more than about .005 radial depth at no more than about 2,000 rpm and 15 IPM or switch to a 3/8 end mill.

You are probably using a 1/4 inch end mill because it's less expensive than a 3/8, but I think you have reached a point of diminishing return.

i run a 3/8 3 flute YG end mill 3500 RPM and 25 to 30 IPM with a radial depth of cut .015 to .025 and i will ALWAYS take at least one spring pass because there is always cutter deflection with small cutters.

[Steve Seebold]

A few suggestions (I'll number them to make them easier to ridicule )

1. Do you know the helix angle of the bit you're using? A higher helix angle may reduce chatter. I accidentally recorded a video where I ended up comparing some tools with different helix angles. The tools also had different coatings and were from different manufacturers, which I realize makes for a poor test, but when I started I was just intending to record the performance of a single bit. Only after it started squealing like stuck pig did I end up changing to other bits. And it wasn't until I was done with the part and started editing the video that I realized the helix angle was probably the most important change.
I guess I should actually link to the video...
https://www.youtube.com/watch?v=CyNkCqthtog

2. I'm going to guess you're doing climb milling. You might consider conventional milling as apparently the angle of deflection varies between climb and conventional milling. That's what this CNC Cookbook article says anyway: Climb Milling vs Conventional Milling
(Look for the Tool Deflection and Cut Accuracy in Climb vs Conventional Milling section if you want to skip straight to the part I'm referring to.

3. You may actually get better results if you increase the WOC. With only 1.5 thousandths to bite on, your cutter might be making some super tiny/thin chips, which aren't ideal. I'd definitely recommend bumping this up if you switch to conventional milling (~10 thousandths (0.010") or so is prolly good).

4. Check out the feeds and speeds recommended by the nifty calculator CNCZone member Bryan Turner made. I plugged in your numbers (I think I got them all) and hit the button to turn the inputs into this link right here
Hopefully that works. I bumped the deflection down to 0.0001". Click the "Compute" button a few times to get more results.

The biggest problem I see is your ER 20 holder. It's just way too long for what you're trying to do. I would have used a 1/2 inch set screw holder to get the cutter as close to the spindle as possible.

[Hirudin]

The biggest problem I see is your ER 20 holder. It's just way too long for what you're trying to do. I would have used a 1/2 inch set screw holder to get the cutter as close to the spindle as possible.

Don't worry about me, that video is almost 2 years old. The point is, all three of those cutters had roughly the same stickout and they were all in the same tool holder and used the same collet and they used the same gcode. Increasing the helix angle eliminated the chatter.

[keen]

A direct into R8 collet will help a little also.

Keen

[Bryan Turner]

Hirudin - thanks for the plug! ;-) Reminds me I need to upload the version with stable-search (so links like that always show the same result).

As for long endmills, I don't see any reason not to try. I use a 1/8" endmill 1/2" deep almost every day (4 diameters deep) - and it requires a stickout of 3/4" to reach the bottom of the pocket. Works great when you get the feeds and speeds right.

Somewhat obvious, but worth mentioning:
- Fewer flutes - try 2 flute (makes the endmill stiffer)
- serrated rough/finish endmill (makes smaller chips, so there is less force pushing against the endmill)
- indexed (helps reduce vibration caused by the rotation of the cutter against the material)
- variable flute (helps reduce vibration along the length of the endmill)
- high helix (lowers the force needed to draw off the chip)

--Bryan