[Jim27]

Looking to mill some pockets in 4140PH and have some corner radius of 0.200 to depth of 0.500 which means a small diameter cutter. Plate is actually 0.500 and holes clear through so not actually pockets I suppose. If needed I could fixture and mill some from both sides but I need smooth walls. Saw some on using boring cuts rather than side milling - seems like a good plan using either an end mill or a drill (undersize) doing the corners first to avoid flex. Might be able to increase the radius min to 0.250. Planning to use carbide 4 flute end mills. I know one option is to go to higher flute count but hoping to avoid that unless really needed. Is 2x diameter reasonable in this material and what sort of chip load and techniques?

[joeavaerage]

Hi,
I'd do two operations:
1) Adaptive clearing with a good quality tool, maybe 5/16 or 3/8 diameter. Leave about 0.5mm radial 'Stock to Leave'
2) Contour with a smaller diameter tool, diameter small enough that it can get into the corners with the radius that you want.
This later toolpath will be you finish path and so you must choose your feeds and speeds and DOC etc to get the finish you require.
With a small diameter tools you will have to be patient as tool flexure will degrade accuracy and finish.

Craig

[Jim Dawson]

With a corner radius of 0.200'' you should be able to use a 3/8 end mill (0.187 radius) at full depth. To get a smooth surface, I normally use a spiral down ramp with about 0.010'' stepover (left from your radial Stock to Leave). Around 0.001 load.

[Jim27]

With a corner radius of 0.200'' you should be able to use a 3/8 end mill (0.187 radius) at full depth. To get a smooth surface, I normally use a spiral down ramp with about 0.010'' stepover (left from your radial Stock to Leave). Around 0.001 load.

This isn't as bad as I was thinking - I was confusing radius with diameter so the tool can be bigger than I had been thinking. For the finish pass is that 0.010" step over and 0.001" load per tooth at full 0.5" depth? If I need to mill the outline with full width and ramp what sort of depth and feed rate would be reasonable? Time isn't a big issue so want to be conservative. It's a large cutout so clearing the whole area isn't practical. Another concern is how to clamp the inner piece so it doesn't more and cause issues when it is cut free.

[Jim Dawson]

Let's start with your machine. What machine do you have?

I would normally bolt the center section to a backing plate with a couple of cap screws.

Here is an example of one part I made using that method. In this case the material is MDF, but the same technique applies in aluminum or steel. In this case it's in my vice, but bolting it directly to the table works also.


Here is another example of work holding bolted to the table, the large screws connect to T-nuts in the slots. The smaller screws are drilled & tapped into the MDF, it could have been bolted to an aluminum backing plate rather than MDF. This started out as a 6x24x0.5'' piece, mild steel.



Full depth, 5 IPM, 1/2'' HSS roughing end mill. Tool path planned so the loose piece on the bottom right would be released without any problem



I'll answer your other questions when I know what your machine is.

[Jim27]

Bridgeport 2216

[Jim Dawson]

Bridgeport 2216

OK, these are the parameters I would use on my machine and should work on your also.

Rough out the interior:

3/8, 4 flute carbide endmill, if possible use a roughing endmill.
About 120 SFM ~ 1200 RPM
5 IPM = chip load of 0.001''
Ramp down to full depth, about 1/8'' step down/pass. I can't give you the ramp angle without knowing what the ID is.

This should be a pretty conservative on a full width cut.

Finish Pass
3/8, 4 flute carbide endmill
About 120 SFM ~ 1200 RPM
7 IPM = chip load of 0.0014''
0.010'' stepover.
Ramp down to full depth, about 1/8'' step down/pass. I can't give you the ramp angle without knowing what the ID is.

[Jim27]

It's a somewhat irregular shape but has flat sides of about 8" on two sides, 4" on one, and an irregular shape on the other. I would think the ramp would best be done on a long straight side if for no other reason than it is easier to think about.

I can easily bolt down the center. So simple it should have been obvious.

[Jim Dawson]

This is what I mean by ramp. This particular part is 1'' thick, and about 6 inch diameter.

This illustrates the finishing pass on the OD. It would look about the same on the ID. A spiral down. It doesn't matter if the part is round or a rectangle or some arbitrary shape. The tool path would feed down at about the same rate. In this case the tool makes 4 passes while ramping down at about 1/4'' down per pass. In this case it is a 1 degree ramp, for less stepdown per pass use a shallower ramp angle, 0.5 degrees maybe? You set this in the Linking Tab.

[machinehop5]

...or another way is to drill the corners out with same drill used for 3/8" bolt down cap screws and use a nice ridged 1/2" 4FL cobalt roughing endmill for full depth 1 pass rough out.
https://www.mcmaster.com/end-mills/r...are-end-mills/
Less problems with chip/swag clearing and coolant flow,. Finish with carbide or HSS 3/8" EM in the G42 direction for nice surface finish.

Just a thought from another machinist,
DJ

[Jim27]

This is what I mean by ramp. This particular part is 1'' thick, and about 6 inch diameter.

This illustrates the finishing pass on the OD. It would look about the same on the ID. A spiral down. It doesn't matter if the part is round or a rectangle or some arbitrary shape. The tool path would feed down at about the same rate. In this case the tool makes 4 passes while ramping down at about 1/4'' down per pass. In this case it is a 1 degree ramp, for less stepdown per pass use a shallower ramp angle, 0.5 degrees maybe? You set this in the Linking Tab.

I see. I was thinking the step down would be over a short distance but I see it is over the whole path.

[kikatorres]

It's not as bad as I thought it would be.