I wonder why ...

[John TenEyck]

I can only get precise 90 deg edges when using an upcut endmill? When I use a downcut endmill I always get a taper, outward, from top to bottom. Doesn't matter if I use a conventional or climb cut, doesn't matter if I add a separate last pass of 0.002 to 0.005", in the same or reverse direction. But if I use an upcut endmill I get exact 90 degree edges.

It happens on both ends of a board, so it can't be related to tramming. I don't think it's runout on the Makita router, either, because upcut endmills give me 90 degrees. The only thing I can conclude is that it's related to bit flex, but I don't understand why. Both bits are new, and both are 1/4". Dust extraction seems about the same for both bits, too. I don't get it. Anyone have any insights?

John

[Jim Becker]

Could be related to the down-cut pushing the material down and introducing just enough stress to deflect it outward as you go deeper. But I agree it's kinda strange! Does altering depth of cut for each pass make any difference?

[John TenEyck]

Could be related to the down-cut pushing the material down and introducing just enough stress to deflect it outward as you go deeper. But I agree it's kinda strange! Does altering depth of cut for each pass make any difference?

I haven't explored that option, Jim. I'm using a 0.15" DOC at 80 ipm on a 1/4" bit, which is pretty pedestrian. Aggressive for me is 0.21" DOC at 120 ipm, still far below what many (most?) people run. Funny thing is the chips seem to be cleared out just as well with the DC as the UC bit, so it must be what's happening right where the bit it is cutting. But it's still strange that it always deflects outward from the top edge of the part. I say strange because the bit is trapped in the cut; it should have no tendency to go left/right except by bit flex and/or runout. The fact that UC bits give 90-degree edges suggests it isn't runout. That brings me back to bit flex and I would think the degree of flex would be related to climb vs. conventional cut direction but it's too small for me to see a difference; both directions result in wedge shaped edges with the DC bit. I tried two different DC bits and got the same result. I get the same result in plywood and solid wood.

This is a major problem for me in trying to use the CNC for furniture quality work. I suppose I could put the parts on my shooting board to true the ends, but that's not something I expected to be required of parts coming off the CNC.

If I look into DOC, do you have any suggestions?

Thanks,

John

[Michael Burnside]

I'm with you John, first thought is bit deflection. With downcuts, I assume you're using a ramping tool path? That's very important with downcut bits, otherwise you'll get deflection, chatter and sometimes breaking. Next thing I'd check is chipload. Make sure the chipload is about the same/identical.

I know runout in drill presses can be exaggerated by excessive heat due to load, but I still doubt in your case runout would be the cause.

[John TenEyck]

I'm with you John, first thought is bit deflection. With downcuts, I assume you're using a ramping tool path? That's very important with downcut bits, otherwise you'll get deflection, chatter and sometimes breaking. Next thing I'd check is chipload. Make sure the chipload is about the same/identical.

I know runout in drill presses can be exaggerated by excessive heat due to load, but I still doubt in your case runout would be the cause.

I'm not using a ramping cut. I can see how that might affect the cut as the bit plunges but why would it cause problems once it moves? Never thought to look into that.

The chipload is the same for both the DC and UC bit, 0.004". Both are two flute running at the same speed.

John

[Michael Burnside]

Hard to say, but 100% you need to ramp downcut bits, always. Depending on the piece I usually try for 4x-8x the bit diameter, so roughly 1-2". I do mostly furniture/hardwoods and generally I have ample runway for the ramp. I usually run my chip loads/DOC at 2x what you are, so I don't think runout or DOC is the problem, but let's start with a nice ramp and see how it goes. Also check your plunge rate. Shoot for something around 50% of your feed rate, or even maybe a little slower.

[Gary Campbell]

Here comes the unpopular opinion:
If some sort of deflection is occurring, it is most likely the machine, not the bit. For the most part, carbide bits don't deflect with excessive lateral force, they snap. The common speak definition of deflection is: "The machine's inability to control the lateral force of the cutting tool". Due to it's chip packing properties, the forces generated by a downcut bit are always higher than an upcut but at the same feeds and speeds.

According to engineering sources the maximum deflection from a carbide bit will be .0016" at 8 times it's diameter overhang. (See chart below) For a 1/4" carbide bit, that would be 2" exposed from the collet. And that number is 16 ten thousandths or 1.6 thousandths of an inch. An amount not noticeable to even the most accomplished operators eye. And that is 16 ten thousandths over 2 inches, which would yield only 6 ten thousandths across a 3/4" material thickness. So, to the guys that speak of "7 to 10 thousandths of bit deflection" on their small or self built machines, I call "shenanigans!"

BTW, that "bit deflection" urban legend was propagated by builders of lower cost, consumer grade CNC machines and bolstered online by the DIY crowd, as it is easier for us humans to find a fault with something other than our own work product. Not to say that some small diameter bits cant deflect, but for the most part, bit deflection really only occurs in milling machines.

Here is a link to an article: Tool Deflection & Its Remedies - In The Loupe (harveyperformance.com) (https://www.harveyperformance.com/in-the-loupe/tool-deflection-remedies/)

And the chart:

500943

To answer your question about why it would deflect most near the bottom of the material, I would say that more extension of the Z axis would contribute to slightly more deflection, which causes the bit to rub on the sides of the channel, which increases force, which increases deflection, and on and on. Compare the 2 sides of the cut. Depending on cut direction (climb vs. conventional) one side will be slightly stepped and the other not. Also, if the "not" side is angular against a square, it is most likely that the Z mechanics are racking, if not, the X and or Y.

[Michael Burnside]

Insightful reply Gary, thank you for the interesting data.

[eugene thomas]

I think gary kind of nailed it ....

[John TenEyck]

Thanks Gary. Here's a photo of the parts cut with a DC bit and another set with a 0.15" deep cut with a DC, and the remainder with an UC bit.


https://lh3.googleusercontent.com/pw/AJFCJaWs8QhVf2K1c1NETPr-XbJ3CRMV5ssatrnviXu9rs6CrLG9ZXMBC2ARVHgn-fSWF6ToDnEXi2rHIIaxdMxjUojLEOUdKvfh7ZdNa2_8AUUDfBX rRDe4JXpUCdvTeaI3ByC1nkDWW2S5l9pZQZQ6p1siqw=w1586-h893-s-no?authuser=1


Here's a photo of a final part, cut with the same DC/UC strategy, showing how the edge is a perfect 90 degrees.


https://lh3.googleusercontent.com/pw/AJFCJaVxKvTGEMZ56NJv60hjCacVT1Cz3rYR4mn88mkNmk0z4N 0kum8nvssj6adxjLvI7haio_-kZErytYqPVOo76w46vQ_SdO2WOdwJCC8yHqdwlH66UF4OIAmxd PyGJMx1emDFd9fkBAq-03X_pTXlmcdhdA=w1586-h893-s-no?authuser=1


Using the square against the side of parts cut with just the DC bit I calculated that the edge tapered about 0.002" from top to bottom, and it's definitely noticeable, especially when you put two parts together. Here's the bad and good:

https://lh3.googleusercontent.com/pw/AJFCJaWs8QhVf2K1c1NETPr-XbJ3CRMV5ssatrnviXu9rs6CrLG9ZXMBC2ARVHgn-fSWF6ToDnEXi2rHIIaxdMxjUojLEOUdKvfh7ZdNa2_8AUUDfBX rRDe4JXpUCdvTeaI3ByC1nkDWW2S5l9pZQZQ6p1siqw=w1586-h893-s-no?authuser=1


And the final parts cut with the DC followed by an UC bit:

https://lh3.googleusercontent.com/pw/AJFCJaVPUl2OWB5cyli4YVwMZp-Ran4SZo0p2-YqODqm_liVpYSdWQ9MjeK2YZFozCTAjjWqkZ3SLwq0B0axGKDo 3jY4XHBH-mIOP-I8vXt7z2Nn2FFfHrwDd7At3kldmzFnZvnFa9SlXkr0pSsT4An_ pV7Ucg=w1586-h893-s-no?authuser=1


They look even better than with the plywood specimens, maybe because the grain is more consistent?

Your chart shows it can't be bit deflection, it would only be 0.0008" over the 1.5" extension I had. So it must be the machine or perhaps the workpiece flexing on the tape/CA glue. Both would be driven by higher lateral forces coming from the bit. If we assume that's true, how much lower cut speed would I need to run a DC bit to eliminate the problem, 20%, more? I can find out empirically, of course, just hoping you might have some guidelines to follow. Thanks.

John

[Gary Campbell]

John....
When I feel that excessive chipload may be the cause of an issue I always recommend to cut feedrate in half, check results and then increase feeds to the max you can and still get tolerable results. That said, if you have something loose, like a bearing block or vroller the issue may persist even at lower feedrates.

Do some push/pull tests on the spindle in all directions to see if there is movement, how much and in which direction. Remember that .008 is probably not visible to the naked eye, so use a dial indicator

[John TenEyck]

John....
When I feel that excessive chipload may be the cause of an issue I always recommend to cut feedrate in half, check results and then increase feeds to the max you can and still get tolerable results. That said, if you have something loose, like a bearing block or vroller the issue may persist even at lower feedrates.

Do some push/pull tests on the spindle in all directions to see if there is movement, how much and in which direction. Remember that .008 is probably not visible to the naked eye, so use a dial indicator

I put a dial gage first on the router collet nut and applied maybe 10 lbs force against the router body in X and Y. I saw about +/- 0.004 - 0.005" in both directions. I got the same results when I applied that force to the Z-axis carriage. And I got about the same results (maybe only +/- 0.004") when I measured directly against the X axis gantry itself, the block that holds the Z-axis.

You were absolutely right.

The 1F is about the most rigid consumer level CNC available. I can only imagine how much flex there is some of the other ones. Unfortunately, the flex is not related to the router, or the Z-axis carriage. It's the X-Y axes and there's seemingly nothing I can do about that.

The only solution I see to getting "perfect" 90 deg edges is to empirically determine what feeds, speeds, and bit combinations work. Oh joy. But at least I have one set of parameters now that works.

Thanks very much for helping me diagnose the root of the problem.

John

[richard newman]

Gary's explanation makes sense, except for the fact that you got the same taper result with a final skim cut of .003" - .005". There would hardly be any chips at all, so chip packing can't be a factor. Just to eliminate all variables other than the bits, have you tried taking a skim pass with both and compared them?

I would also check to make sure the down cut bit isn't itself tapered. Stranger things have happened...

[Gary Campbell]

Gary's explanation makes sense, except for the fact that you got the same taper result with a final skim cut of .003" - .005". There would hardly be any chips at all, so chip packing can't be a factor. Just to eliminate all variables other than the bits, have you tried taking a skim pass with both and compared them?

I would also check to make sure the down cut bit isn't itself tapered. Stranger things have happened...

Can't comment on a bit being tapered, but have never seen one that is, that was not designed to be. That said, the reason the taper exists when using a (same direction) skim cut is that the higher load moves the bit away from the intended cut path and a final skim cut will usually be right on it. For example when using a ShopBot for cutting cabinet parts I would 3/4 ply cut at ~400 ipm down to a skim cut climb direction and then follow with a finish cut ~.030 conventional, which left the part ~.005-.010 undersized with a good edge. Careful examination of the waste would show a .030 wide, .030 high step at the bottom edge.

[John TenEyck]

Gary's explanation makes sense, except for the fact that you got the same taper result with a final skim cut of .003" - .005". There would hardly be any chips at all, so chip packing can't be a factor. Just to eliminate all variables other than the bits, have you tried taking a skim pass with both and compared them?

I would also check to make sure the down cut bit isn't itself tapered. Stranger things have happened...

I did use a skim cut, called a last pass cut, in VCarve Pro. It helped but did not eliminate the problem with the DC bit, but it works very well with the UC bit. I'm using a pass of 0.002", doesn't need more. I'm using a climb cut for all passes. I tried using a conventional cut for the last pass and that left a very chattered surface on the ends of the parts where it's cutting cross grain.

For one-off work, it looks more and more like conventional methods work better for making furniture related parts.

John

[Michael Burnside]

Man, 400 ipm and basically one pass. That's cool. I usually run in the 200-250 ipm range and 2-3 passes, LOL. I think I have my plywood chipload setup somewhere around 0.01"-0.012" depending on species of the veneer. I build furniture though, so I usually try to pick something that keeps good chipload and little to no tearing. Maybe I'll try something a bit more aggressive on the next shop project and see what happens.