Machinist-CNC toolpath help

Wondering if any of you pros can help me.
On stainless (300 and 400 series) and carbon (1018) steels I'm getting a loud squeal during the helix ramp into the material. Once at the correct Z depth the endmill runs great, it's the initial ramp that is giving me troubles. Default in Fusion 360 is a 3 degree ramp, I've tried up to a 7 degree with the same thing happening but less time duration due to the steepness of the ramp. I'm using 4 flute carbide endmills ALTiN coated, shortened up as far as I can go with ER32 CAT40 holders 1.85" long which is the shortest you can get from Maritool. Most of the time I'm using a .50" EM but the same thing happens on .375" . Helix feed is the same as the cutting feed. Again once into the material everything run fine. Feeds and speeds I'm getting from the G Wizard application. Most of the time I'm using a mid range value between conservative and aggressive. Workholding is a Kurt 3600V.
Any help is appreciated
Edit: I also tried increasing/decreasing the feed rate and spindle speed at the controller in 10% increments with marginal success, sometimes worse

 

Go to a 2 flute or 3 flute. I'd try a 3 flute. It'll be a tick more rigid. Any thru holes it might not be a bad idea to pre drill and then bring it out to size with the end mill.

 

All of my stuff is ancient manual equipment so my experience with your issue is nada. However, typically when I get the squealing sound you describe it is either from to much or to little chip load. Since you say the cut is fine at full depth is it possible that during the ramp phase you cannot get enough chip load to prevent what is most likely chatter?

There are times with my mill which only has a max rpm of ~3300, so slow, when taking light cuts in AL that I haven’t found a way to not have some chatter other than trying to have my feedrate as high as I can crank the handle.

 

A 2 or 3 flute would increase his chip load if entering at the same feed rate and RPM as the current 4 flute so that may be a benefit on entry as well.

 

Could be any number of things. Your pic is named Haas so I assume you're using coolant... is that true?

I wouldn't use a 2 flute with stainless, 3 flute may work though.

The comment about chip load is probably the ticket, try increasing the feed rate on the ramp (assuming you can, I don't have experience with F360), I'd start somewhere around 1.5x where you are now, and work up if you need to.

Maybe also try a linear ramp in instead of helix? Helix is ideal because you're not shocking the tool, but give it a shot and see if it changes.

 

Most endmills don't like to ramp. Even if they are "center cutting". The problem lies in the end relief or angle of the cutting edge on the end of the cutter. The squeal you're hearing is the end of the cutter rubbing as it's plunging. Your ramp angle needs to be LESS than the relief angle of the cutting edge. Rubbing is one of the most common types of tool failure, and the one that causes people to scratch their heads the most because it's sometimes counter intuitive.

You can buy special end mills (I'm in holiday brain cell killing mode, so the name escapes me at the moment) designed for high ramp angles and it's very obvious looking at the business end what they are designed for. Most normal end mills will live a long happy life ramping at 2-3*.

Edit: sometimes tools just squeal, or are noisy during certain parts of a toolpath. It can drive you nuts chasing the source, and trying to find solutions to stop it, but as long as tool life isn't suffering and surface finish is ok then that's what they make earplugs for. We have long roughing tools that are very noisy and squealy in corners, but other than that are perfectly fine. Just the nature of it.

 

I can bump up the feedrate on the helix only if needed, I'll try the 1.5x you suggested as a starting point. I also tried zig zag on one part .25" EM on a slot .30" wide and got similar results with the squeal.
I am using coolant
Thanks

 

These are square endmills, no edge radius.
Surface finish is great, usually do my roughing passes at multiple depths leaving .01" stock to leave and a full depth finish pass at a slower feedrate

Here's an example piece I recently did. The oval is 1" wide, material is 1018 steel, 1" thick. Used a .50" EM on the oval, chipload was .0018" per tooth

 

The shop I worked at got rid of most of the 4 flutes, switched over to 3 flute quick twist or hi Helix. Why aren't you pre drilling the slot.

 

What brand of beer are you holding while the is running? I've found switching to a different beer, or maybe scotch or bourbon, will cause machine problems to go away.

Well maybe NOT go away, but eventually you won't care so the end result is the same.

Or maybe you need a henweigh for your workpiece.

 

If you look at the primary relief angle highlighted by the red line, You can't increase your ramp angle (blue line) beyond that without rubbing it for part of the cutters rotation. That's where the squeal is coming from. It's not related to corner rad, center cutting/non center cutting, chipload (sometimes but not in this case) or anything else. You need a couple degrees of relief behind the cutting edge to prevent squeel (rubbing induced vibration).

 

Dude, you know your stuff...

 

So you are saying that even though the tooth is removing material that as it ramps down the cutter is still prone to rubbing at the trailing side of the cut. I may not have stated that correctly but I do understand relief angles at it pertains to drill bits and why it needs to be there.

 

Essentially yes. The 1/4 of rotation when the cutting edge is plunging steeper than it's relief angle is causing the backside of the cutting edge to rub and cause vibration. It only happens for a minute second until the cutting edge rotates OUT of the "plunge" but it happens. Grab an end mill in your hand and spin it slowly to visualize the different stages of cut as you plunge and it should be easier to visualize.

 

I didn't read all of this, but NEVER do hard roughing in a collet. Always use a solid holder.

And 4 flute only on anything steel

 

Thanks for the explanation Dan, that makes sense to me. I'll go to a shallower ramp angle next time

 

Try to use a heat shrink or solid endmill holder for the rougher. Unless that is a high performance endmill your surface speed looks pretty high to me for 400 series stainless. General purpose tools are normally going to fall between 200-250 sfm.

 

That example was for 1018 steel

 

The picture in the original post looks like an ER16 but your post states an ER32. Just making sure.

Post a closeup pic of the part / work-holding and the tool-holder you're using and we might be able to see where the squeal / chatter is coming from.

I'm not trying to be disagreeable but... I rough in Titanium using an ER32 all day long with no issues. Works just fine.

Again, depends... 4-flute is great in steel but so is a 5-flute or even a 6-flute if you want to take a smaller bite or are machining stainless or nickel steel alloys. A smaller radial DOC while hauling the mail in terms of RPM can get you some great metal removal rates and nice finishes. A 6-flute Destiny Raptor in stainless can be amazing.

 

This is some solid info right here. The only thing I’ll add is I’ve never liked ramping or plunging with anything more than a 3 flute when using 1/2” endmills.

I’ve even went so far as to drill a start hole and plunge in at the hole with 4 or 5 flute endmills but, then again I’ve been out of the metal side for a while now except when I’m doing stuff at home for fun on my HAAS.