Ridges at bottom of pocket

[martin54]

Hoping one of the experts might be able to point me in the right direction, i sometimes get a ridge at the bottom of a pocket but there doesn't seem to be any consistancy as I would expect if there were a repeatable problem.
If you look at the ridge on the first brass it is clear where it has happened but there are absolutely no lifts in the machine cutting & nothing I can see or hear o give any indication why this might be happening. If you look at the second brass you can see that there are no ridges what so ever & the 2 brasses sit side by sie on the same piece of flat bar. Both were cut at the same time with the same type toolpath & same bit.

[4DThinker]

My first guess would be that your spindle isn't perfectly square with your bed. I bit that is slightly off vertical will leave ridges.

4D

[mtylerfl]

Wow! Those are fairly severe!

Try an Up Cut Bit with a smaller stepover (40% or less), after you have verified the tram of your router. I’m also wondering if the feed rate is set too fast and contributing to the chatter/marks. What’s your Pass Depth? - might lessen that, as well.

Lots of shots in the dark without seeing your file and being present to witness and listen during cutting in the first place.

[TReischl]

Martin, are you taking a light finish cut after roughing?

Another question, are you ramping your cutter to depth on plunge moves?

Something is gnawing in the back of my mind about putting stress on a collet that is not top notch and then strange intermittent problems start showing up.

IIRC, you do not use router collets. Seems to me you use ER collets on your machine.

[Leo]

That does look pretty severe.

If the spindle was out of tram the marks would look very different than what I see there.

That looks like some heavy chatter. Too fast on the RPM can do that, but also many other things as well.

The 3D cutting on the deer looks pretty good.

Can you be a lot more specific on the cutting parameters, RPM, DOC, Feedrate, cutter geometry, 2 flute, ball nose, stepover - all that stuff. Did you use any cutting fluid? How well did you clamp the workpiece? How far was the cutter sticking out of the collet? What sort of collet did you use? All of this can attribute to cutting performance.

[martin54]

I should know better than to provide only half the details

my own view which could obviously be wrong is that if the spindle were not trammed correctly then I would get those marks in he second picture as well as the first.

Speed & feed settings, 16,000 rpm, 70imp feed 65 imp plunge rate, DOC 0.25mm (0.0098 inch approx) brass CZ121 free machining brass cut dry, no cutting fluid at all.
End mill, standard length 2 Flute AlTiN Coated 45HRC, 3mm diameter on 4mm shank, approx 20mm (0.7874 inch) stick out, kept it as short as I could without clamping on flutes.
ER 20 collet chuck, 4mm collet not the most expensive so run out isnt super accurate, it has done a fair bit of work but hasn't been abused & gets cleaned after use as does the collet nut.

This is a standard pocket cut, I always ramp rather than plunge the ramp for this is over 25mm (approx 1 inch) oth pockets are same depth cut in the ame number of passes. No it's not a final finish cut Ted you are right about the collet chuck lol

[garylmast]

My guess would be the mill is slipping down or out of the collet (bad or worn out collet) or the mill may be dull or clipped.

Gary

[mtylerfl]

Ha! I just recognized the Fox! I created that model many years ago. It used to be for sale at VectorArt 3D before it became Design & Make.

For a second, it looked like you also had a Hummingbird model I created too, but I can only see partial wings and the tail doesn’t look like my hummingbird model.

I believe that particular Fawn model was created by James B., way back when...

Say, one more thing to check regarding the chatter marks. The Bit itself...check the end to make sure it’s intact (no chunk broken off).

EDIT: just noticed Gary beat me to that idea

[martin54]

I did wonder about the collet, actually have another one on order but not arrived yet but didn't think that was really the problem as I would have thought that would show itself on the plunges when the bit moved to a different part of the pocket. This has happened on a part of the pocket where there is absolutely no lifting of the z axis, purely X & Y axis movement, the cutter appears to be good from what I can see, still seems to be sharp, it was a new bit at the start of the job & the fawn was cut after the fox.

Design & make now sell that fox model Michael I bought a couple of models for this job as the 3D models looked much nicer than the raised outlines, well I thought they did anyway lol, I would have bought a couple more but they came out of my pocket & I simply can't afford any more just now.
The wing you can see is from the mallard in the wildlife scenes duck panel. I was going to use one of the Deer from the wildlie scenes collection but these are quite small & the antlers were giving me problems with machining so I went for the fawn instead.

[highpockets]

Martin,

One more thing you might consider, because the ridges are showing up in what looks to be random areas the brass you are using may be warped just a tad causing flex in the material downward as the cutter passes over some areas causing the cut not to be at the right depth then when the cutter gets to an area where the mass (body of the fox) the cutter is milling at the correct depth, causing the ridge. I'm guessing you're already pulled the piece from your table, but if you haven't you might try using a dial indicator to check for warpage. It could also be some flex in your table. I also noticed that the piece you're showing that you're having problems with is in the middle of the piece of brass. How are you ensuring it's not lifting?

Metal is a lot more ridge than even hard woods, so an issue in metal might not have shown up in milling woods.

Just a thought.

[martin54]

No it's still on the machine John Got another couple to fit on this length of bar before I take it off, it's 3/16 brass bar & I haven't surfaced it so yes you could be right about it not being completely flat, I didn't think the cutter would be enough to push it down but you might be right.
Flex in the table is very very unlikely Have you seen my machine? It's very heavily over engineered for what it is, think Gerber must have realised that as latter machines have a much lighter frame

Sorry people forgot to list the stepover when I gave the details & it won't let me edit the post now. Step over is 15% I believe, certainly no more as I was a little concerned about the finish on the bottom of the pocket, if it isn't 15% it will be 12%

[Leo]

The RPM's seem a bit high. Routers don't like low RPM's but I try to get down to 5,000 or so.

DOC is light, but OK. Hopefully the machine is very rigid.

The pictures are not really all that clear, but it looks more like chatter than a spindle out of tram to me.

The stick out is good

One thing we find at my workplace is that a VERY sharp cutter and a VERY high rake cutter does a much better job on soft metals like brass and aluminum.

Perhaps a high helix not coated will work better. High helix would be a 60 degree helix. Or an end mill specifically designed for aluminum cutting. Coatings can tend to dull the sharpness of the cutting edge. Or perhaps a HSS uncoated end mill. Some people claim that HSS can be sharper than carbide.

[martin54]

I won't get down that low Leo, below about 6000 rpm my spindle doesn't have enough torque to cut butter, warm butter at that

I thought the DOC might be a little bit low but as I have said in the past I do tend to be conservative, probably to much so to be honest. What would your figures be for a 3mm end mill (2 flute) & a 1mm ball nose? I know it is always machine dependant but my machine is pretty ridged, t's an old production machine, Gerber system 48, electronics have all been replaced but still oriinal mechanically (well almost) fitted a chinese spindle & VFD in place of the original Porter cable router because the router was BER & in the UK they are more difficult to get hold of

[Leo]

Looks like the ball nose is working OK. I have used cheap chinese ball nose on brass for 3D and it was good.

I would need to play around with the 2 flute. First, use a NEW cutter, uncoated. If you can get a cutter for aluminum - SKI CARB or something really good. If you get a stubby end mill - even better.

3mm is pretty small. That could chatter just because it is small, and I think you said 20mm stickout - that not a really good ratio. A stubby tool would be better. Is it at all possible to use a larger diameter tool - as large as possible - would be best. It you could get a 1/2" cutter you would be WAY better off. One nice thing about Vectric is the solid toolpath preview. Try larger tools and see what you can get. Even use the larger clearance tool in the pocketing and use a 3mm to just clean up the leftoner stuff.

The .010 DOC is ok - depends on the rigidity and power of the machine.

Next - get accustomed to calculating chipload. The combination of RPM and Feedrate is all you need to play with to get the combination for your machine.

Try for .0008 - .0012 chipload
This way you can adjust your feed or RPM accordingly, and keep chipload constant.

This calculator does not display below .001, so it is not really optimal
https://www.guhdo.com/chipload-calculator

If you want I can make a calculator that will display to .0001 if you like.
I can email the excel form for you

Brass doesn't really need coolant, but, like chicken soup, it could not hurt. Cool Tool is a cutting fluid that you can get is really small plastic bottles and just drip around the cutter. Personally to me it doesn't do much more than make a mess, but it will not hurt. You can use WD40, but it's not really a cutting fluid

[martin54]

I will play about some more, it was a new bit but it's coated, I do have high helix cutters for aluminium but not that small, the 3mm bit IS the larger area clearing tool should have used something for scale but these are only 4 inch square lol
First tried a 6mm cutter but that left far to much for the small tool to clean up, then tried a 4mm cutter which again left quite a lot uncut so the 3mm seemed to be the best option

If the conversion on the denford triac were done then I would be using that to cut these Unfortunately that will have to wait until I have saved up a bit