Slot cutter - chatter issues

We are running a 1.970” diameter, 12 flute solid carbide cutter mounted to a 1” HSS shank. The cutter is .236” wide with .094” radius on both corners.

We are cutting a slot that finished at .406” wide with a 1” radius.

The material is 4340.

We are having trouble eliminating chatter. We are climb milling on a WFL Mill turn. We’ve tried .01” radial DOC for finish pass, we’ve tried .005” radial DOC for finish pass. A spring/free pass seems to help. HSK100 tool holder, the part setup is relatively rigid. The finish looks great on the exit of the tool path but chatter on the entry. It’s cutting a straight line to an arc to a straight line.

Do you think conventional tool path would help?

I don’t have much experience with a tool of this type. What SFM would you recommend? Chip load? I believe a lot of teeth are engaged in the cut at any given time. How is this determined/calculated?

Thanks in advance for the support.

- Branden

Have you tried adding a horizontal lead-in radius and adjusting your lead in feedrate?

What's your current SFM?

I'd slow 'er way down. Maybe 200 SFM and 0.0008 IPT for starters.

You mention the carbide cutter mounted on HSS dengas end. How much stick out from the "chuck" do you have? How ridged is the set up?

Orange Vise said:

What's your current SFM?

I'd slow 'er way down. Maybe 200 SFM and 0.0008 IPT for starters.

Click to expand...

I should have mentioned that we are running 400 SFM and .0006” IPT. I’ll give these cutting parameters a try. Thank you

doug8cat said:

You mention the carbide cutter mounted on HSS dengas end. How much stick out from the "chuck" do you have? How ridged is the set up?

Click to expand...

It’s a 1 inch HSS shank in an end mill holder and it’s rigid. It’s only sticking out of the holder 1.25 inches. The set up of the part isn’t as rigid as the tool. Thank you

NiCu2829 said:

We’ve tried .01” radial DOC for finish pass, we’ve tried .005” radial DOC for finish pass.

Click to expand...

Have you tried taking a larger cut for finishing?

Mtndew said:

Have you tried taking a larger cut for finishing?

Click to expand...

Yes. It doesn’t like I have a finish pass.

The tool path is a linear move to an internal arc back to a linear move. It was feeding at the same feed rate for the linear moves and the arc. the tool diameter is 1.969” and the finish part diameter is 2.0. With such a small arc and large tool diameter it was feeding to fast on the radial move. I added additional feed rates so that the actual chip load is consistent throughout the tool path at .0027.”

Shouldn’t the cam software accommodate for this based on the radial depth of cut, the tool diameter and the finish part diameter? Does a different tool path have to be selected Within the software?

Have you tried switching holders?

NiCu2829 said:

Yes. It doesn’t like I have a finish pass.

The tool path is a linear move to an internal arc back to a linear move. It was feeding at the same feed rate for the linear moves and the arc. the tool diameter is 1.969” and the finish part diameter is 2.0. With such a small arc and large tool diameter it was feeding to fast on the radial move. I added additional feed rates so that the actual chip load is consistent throughout the tool path at .0027.”

Shouldn’t the cam software accommodate for this based on the radial depth of cut, the tool diameter and the finish part diameter? Does a different tool path have to be selected Within the software?

Click to expand...

What CAM software ?. InventorHSM has feed rate reduction on internal/external arc/corners.