Pocket/Inside Corner Milling Strategies ?

[ColinFitzgerald]

Hi all !

I had a question about milling pockets. I've been using a spiral
outwards type of strategy, but when the end mill moves to the next
spiral, it cuts much harder as its now cutting full width. Same thing
happens when cutting into a corner with a radius close to that of the
end mill. Now if I take things slow this isn't a problem, but if I
try to push the cutter so that its operating near its feed/depth
limits on a normal profile/shoulder cut, the dam thing breaks or chatters when
it tries to cut through a tight corner.

Now the reason this happens is obvious to me (in the corner the
material removal rate goes way up for a brief moment). Whats not so
obvious is how to deal with this effectively. Is there a better strategy ? I
don't much like the idea of lowering feeds/depths just so the corners
cut well.

One idea I had was to lower the feed just in the corner, but since my
CAM software (OneCNC XR2) can't do this automaticly that amount of
manual code editing would be nutz.

Also note, this is really only an issue when roughing.. so I don't
really care about the surface finish or even the accuracy, just don't
want to break end mills.

FWIW, as one example, I was trying to cut 6061-T6 with a 3 flute 1/4" carbide end mill (Robb Jack, standard length). A shoulder cut at 0.25" depth (1D), 0.1875" (75%) width at 4500rpm and 65IPM (0.0048 ipr) works pretty good and sounds like it is at the limit of the cutter. As soon as it hits a tight inside corner, the end mill breaks !

Also, my machine is a Tormach PCNC1100. The 4500rpm and 65ipm is machine max. BT30 spindle, Lyndex SK collet holders. I know the SFM is a bit low for carbide. I'm using Valcool 777, a semi-synthetic oil based coolant.

I read a number of posts on speeds/feeds and I seem to be in the ball park. My problem has more to do with path geometry then feed/speed issues.

Am I just pushing too hard ?

Any other ideas/suggestions ?

Thank-you very much !!

Colin Fitzgerald

[HIRAH]

seeing the limits of your machine, i would say to try drilling the corners out first. at 65 ipm this would take less time than slowing down the endmill in the corners.

[lerman]

Could you spiral in instead of spiraling out? Take the first pass at a lower feed. Then up the feed for the rest of the job.

I've never tried it, but it seems like it should work.

Ken

[DareBee]

Program your part with much larger corner rads for 1st roughing. Then re-ruff the corners with a smaller cutter or the same cutter with a lower feed rate.

[silverfoxx03]

there is a type of cutting that is call trichordial--basically what it does is make extra passes in the corners to remove the material and maintain a constant chip load. Most of the softwares out there have this feature in it, but if yours doesnt, then you really need to reduce your feed in the corners by about 50% to allow for the extra chip load that is put on the cutter when it hits the full engagement. If you can do a sweep into the corners to maintain a constant chip load and then come back and finish the radius with a smaller cutter, that would work also.

Let me know if I can help more

cwilliams@singlesourcetech.com

www.singlesourcetech.com

[fpworks]

Colin,
I think your cutting parameters are right at the limit of the tool...as long as the tool engagement angle is not increased by going inside corner...as you've found. Having said that, your feedrate is just simply too high for the feature you're trying to cut. So yes, you are pushing too hard.

Unfortunately, with your CAM program, you have to limit your cutting parameters with regards to the feature, and this will leave some time on the table.

We switched from OneCNC to a different package last year because of the ability to have high speed toolpaths AND a feed optimizer. (ANY machine can benefit from these more advanced toolpaths) I heard that OneCNC was planning to add high speed toolpaths in the future...not sure about the feed optimizer/high-feed/adaptive feedrates.

In the meantime, if you're really concerned about your cycle times, you will have to manually edit the program to slow your feedrate for the corners. I suggest a program called NCPlot...they offer a demo before purchasing. Also, you could start conservatively, then listen to the cut while watching the line numbers on the control. Take notes, and increase feed rates where it sounds like the tool can handle more.

Anyhow, with this limitation in mind, I suggest using a two flute endmill rather than a three flute for pocketing operations, until you get to 3/16" or smaller, then I prefer a three flute for tool rigidity. With soft and gummy materials such as aluminum, two flute endmills can accept a higher feed per revolution than three flute endmills. Also, two flute endmills like to plunge MUCH better than three flute tools, which can expedite your pocket entry.

Regards,
Justin

[HuFlungDung]

Is the broken off tool typically plugged, or clear of aluminum chips?

I would say you are pushing that tool pretty hard. Perhaps roughing with a larger tool is in order. I will often rough drill some holes to clear material and permit the smaller tools to handle the cut.

If you don't want to do a toolchange, then Darebee's idea is a good one as well.

[Mussel Kar]

If it is a square pocket you can cut an X pattern corner to corner at slow/proper feed. Go back to higher feeds for the rough pocket because there are no corners left.

[eorourke]

I am with Silverfox on this one! Trichoidal is probably the best and fastest technique for removing material in a pocket. It maintains constant chip load so it will give you better tool life. It will also allow you to program faster feed rates since it doesn't put an extreme load on the spindle. This will reduce your cycle time significantly. As Silverfox says, there are a variety of CADCAM programs out there that offer this feature.