To Interpolate or Not To Interpolate?

NiCu2829 · Jan 9, 2019

I've attached the blueprint of the part to be made, photos of the actual part, the drawing of the carbide tool (it’s custom) and actual photos of the tool that I'll use to cut the feature in question.
I'm making this part on a Citizen L32 (Swiss machine). This operation is taking place on the main spindle, in guide bushing mode. The tool is running in an ER20 live tool. The material is 4140.
The tool is 1.000” diameter (.500” radius) and the blueprint calls for a .500” radius so initially I tried plunging the tool to depth. The photos of the part show the results of this, it chattered. I’ve just discovered the tool doesn’t have the proper relief behind the cutting edge (see photo) and is rubbing, causing a heavy burr and excessive tool pressure, which I’d say is contributing to the chatter.
Considering cycle time, I thought plunging would be the preferred method, agreed? Now I’m beginning to think that I should try and interpolate this feature, any thoughts?
Any help/insight will be greatly appreciated!

Dropbox link to photos: Dropbox - ~ Interpolate - Simplify your life

Hazzert · Jan 9, 2019

Just curious, is that tool from Internal Tools?

Comatose · Jan 9, 2019

Any time you plunge a many-tooth cutter into a part the cutting force goes way way up. This is why you're getting chatter: it is easier for the tool and material to deflect away than it is to make the cut you're asking. Once they deflect away, the cutting force comes down, and they move back together. Lather, rinse, repeat. A couple contour passes with a smaller tool will get you better results. You need the smaller tool so you have fewer teeth in the cut at the end. Full engagement on a tool in a corner like this will usually chatter, whether it's a saw type cutter or a regular old endmill.

doug925 · Jan 9, 2019

Comatose said:
A couple contour passes with a smaller tool will get you better results. You need the smaller tool so you have fewer teeth in the cut at the end. Full engagement on a tool in a corner like this will usually chatter, whether it's a saw type cutter or a regular old endmill.

This! (my same thoughts to you via PM)

DMF_TomB · Jan 9, 2019

if plunging with a end mill and i care about surface finish of corner or radius left if possible i will plunge .003 to .005 away to rough out material
.
go back up, move to final position and plunge the smaller .003 to .005 amount. basically take a finish cut of a smaller amount

CarbideBob · Jan 9, 2019

The tool is made wrong. No programing will fix this.
Yes, I know it is a ever other which is why second evey skip but it is wrong.
Send it back and have it modified.
Bob

Hazzert · Jan 9, 2019

CarbideBob said:
The tool is made wrong. No programing will fix this.
Yes, I know it is a ever other which is why second evey skip but it is wrong.
Send it back and have it modified.
Bob

That is why I asked if it was an IT tool. I have bought a couple customs from them and they had a similar lack of relief. We modified it in house and suddenly it started cutting :wall:

garyhlucas · Jan 9, 2019

I gotta follow this thread. I just ground a similar tool on my home built CNC mill. I put 7 degrees of relief on the sides, I hope that is enough. First attempt at such a tool, but I have had decent results with a couple others I have done.

Bobw · Jan 9, 2019

I’ve just discovered the tool doesn’t have the proper relief behind the cutting edge (see photo) and is rubbing, causing a heavy burr and excessive tool pressure,

which I’d say is contributing to the chatter.

Ya think???

Get it cutting right first, by cutting right, I mean CUTTING!! not trying to make a friction
stir weld...

I don't know if you have to send it back or not, if you do, I'd be pissed, I'd be pissed anyways,
shouldn't custom tool makers understand relief angles and the fact that they are making CUTTING tools,
and they need to actually CUT! If I wanted a broach, I'd buy a broach, if I wanted to rub it out :eek:

I'd order a grinding wheel.

I think that proper relief will cure 95% of your problems..

If it doesn't.. Throw a chamfer on the corners. top of one tooth, bottom of the next..
If the chatter is really bad, do 2 consecutive teeth on the top, alternate a few, then
2 on the bottom.. Maybe some grooves in a few teeth, like a rougher.. And if all
else fails, just grind a whole entire tooth off.

But at least get it cutting properly first. And make sure your collet nut is torqued down proper.

Vancbiker · Jan 9, 2019

Hazzert said:
That is why I asked if it was an IT tool. I have bought a couple customs from them and they had a similar lack of relief.

I'm interested to hear if IT made the tool also. I've not used anything custom from them and the stock tools I have gotten from them have worked great. When the time comes I need a custom though, I want to know if they are up to it.

TeachMePlease · Jan 10, 2019

Vancbiker said:
I'm interested to hear if IT made the tool also. I've not used anything custom from them and the stock tools I have gotten from them have worked great. When the time comes I need a custom though, I want to know if they are up to it.

Never had an issue with them. And I've bought a LOT of them.

Next time you need a custom, check with MITGI too, they do nice one offs, and quicker than IT (or anyone else)

NiCu2829 · Jan 13, 2019

Hazzert said:
Just curious, is that tool from Internal Tools?

It is not. Will they make special/custom tools such as this?

NiCu2829 · Jan 13, 2019

Comatose said:
Any time you plunge a many-tooth cutter into a part the cutting force goes way way up. This is why you're getting chatter: it is easier for the tool and material to deflect away than it is to make the cut you're asking. Once they deflect away, the cutting force comes down, and they move back together. Lather, rinse, repeat. A couple contour passes with a smaller tool will get you better results. You need the smaller tool so you have fewer teeth in the cut at the end. Full engagement on a tool in a corner like this will usually chatter, whether it's a saw type cutter or a regular old endmill.

Thank you for the reply, my apologies for the delayed response. I've sent out a number of RFQ's for a tool with 6 flutes and a diameter of .965" this will allow me to interpolate. I wasn't sure whether to plunge initially then interpolate the last pass or interpolate all passes, am I correct in saying that you're suggesting I interpolate all passes?
Your point about the smaller tool, are you referring to smaller diameter?

Thanks again for the support.

NiCu2829 · Jan 13, 2019

doug925 said:
This! (my same thoughts to you via PM)

Thank you for the reply Doug. I've sent out a number of RFQ's for a tool with 6 flutes and a diameter of .965" this will allow me to interpolate.
The point about the smaller tool, are you referring to smaller diameter? The smaller the diameter and less flutes = less tool pressure, correct? However, I'm not sure I fully understand, wouldn't the distance between flutes be greater the larger the diameter of the tool? If so, wouldn't there be fewer teeth in the cut with the bigger diameter tool. I agree that I need a smaller tool with less flutes, I'm trying to visualize. The understanding is important to me.

Thanks for the support.

NiCu2829 · Jan 13, 2019

DMF_TomB said:
if plunging with a end mill and i care about surface finish of corner or radius left if possible i will plunge .003 to .005 away to rough out material
.
go back up, move to final position and plunge the smaller .003 to .005 amount. basically take a finish cut of a smaller amount

Thank you for the response.

NiCu2829 · Jan 13, 2019

CarbideBob said:
The tool is made wrong. No programing will fix this.
Yes, I know it is a ever other which is why second evey skip but it is wrong.
Send it back and have it modified.
Bob

Thank you for the response. You are correct Bob, the tools was incorrectly ground. It wasn't intended to be a staggered tooth tool though. The new/updated/correct version should be at the shop tomorrow. I'm looking for better results, but I agree with others that have responded, interpolation is necessary.
Again, thank you for your time.

NiCu2829 · Jan 13, 2019

Hazzert said:
That is why I asked if it was an IT tool. I have bought a couple customs from them and they had a similar lack of relief. We modified it in house and suddenly it started cutting

Good to know, thank you.

precisionmetal · Jan 13, 2019

Definitely interpolate. It's the best long-term solution, IMO.

NiCu2829 · Jan 13, 2019

Bobw said:
Ya think???

Get it cutting right first, by cutting right, I mean CUTTING!! not trying to make a friction
stir weld...

I don't know if you have to send it back or not, if you do, I'd be pissed, I'd be pissed anyways,
shouldn't custom tool makers understand relief angles and the fact that they are making CUTTING tools,
and they need to actually CUT! If I wanted a broach, I'd buy a broach, if I wanted to rub it out
I'd order a grinding wheel.

I think that proper relief will cure 95% of your problems..

If it doesn't.. Throw a chamfer on the corners. top of one tooth, bottom of the next..
If the chatter is really bad, do 2 consecutive teeth on the top, alternate a few, then
2 on the bottom.. Maybe some grooves in a few teeth, like a rougher.. And if all
else fails, just grind a whole entire tooth off.

But at least get it cutting properly first. And make sure your collet nut is torqued down proper.

Thank you for the response Bob. The tool maker did acknowledge the error and he's supposed to have new tools arriving at the shop tomorrow. I've sent out a number of RFQ's for a tool with 6 flutes and a smaller diameter of .965" The grooves "like a rougher" idea sounds logical, I'm not a tool maker though. I'm looking forward to receiving the tool with 6 flutes. The nut (ER20) is recommended at 22 ft/lbs per the manufacturer and that's where I've set it.
Thank you for your time.

NiCu2829 · Jan 13, 2019

TeachMePlease said:
Never had an issue with them. And I've bought a LOT of them.

Next time you need a custom, check with MITGI too, they do nice one offs, and quicker than IT (or anyone else)

Thanks for the reply. Good information. Typical lead time?

To Interpolate or Not To Interpolate?

Plastic

Attachments

Stainless

Titanium

Titanium

Diamond

Diamond

Stainless

Stainless

Diamond

Diamond

Diamond

Plastic

Plastic

Plastic

Plastic

Plastic

Plastic

Stainless

Plastic

Plastic

Similar threads