Step over 2nd/3rd pass

[Sjotime]

Hi all,

Consider yourself prethanked for looking at this post! I appreciate any feedback assistance you might offer.

THE SETUP
Rhino/Visual Mill/Mach 3

MACHINE
Rebuilt by a friend (far away, so I can't throttle him) with Geckos etc, Digital Tool frame, servos, 3 1/4 PC router, belt drive

THE APPROACH
I cut a lot of 3/4" furniture grade plywood. I do that in essentially two steps.
1. 1/4" downcut spiral bit cuts to 1/4" depth.
2. 1/4" upcut spiral bit cuts to 1/2" then 3/4+ penetrating the piece.
Note: Downcut runs clockwise to the piece, upcut runs counterclockwise.

THE PROBLEM
The upcut runs cut slightly offset from the downcut, usually in one axis. In small parts spread across the table the offset grows incrementally. You can imagine the problems: dimensions, edge finishing, fitting ETC ETC ETC!

TESTS
I cut two squares to test the cut direction setup and the down/CW up/CC approach yielded the best results. Smallest step, square piece, 1/32 off in one direction. NOTE *** Never been trained on CNC. Just bought this thing from my buddy and started messing around. Don't know jack about Gcode and just work the VM the best I can. Is this CW/CC thing even right???

THOUGHTS
Is this a backlash problem? I've got belts, not a gearbox. But everything drives on tracks...
On the physical setup, I've tighted all excentrics, replaced the router (it was time), checked/matched belt tension as much as I am able.

Seems like the bits are driving off course, pulling out of line. It does seem fairly consistent in one axis, but inside and outside curves are problems.

NEXT STEPS
...that I've thought of: backlash compensation. Any clues on setting that up? Standard tests?

Is this electronic? Erf. The mind reels... Any thoughts appreciated.

Or, selling the router and getting out of the 'making stuff for people' business.

Your thoughts/comments are so appreciated. I am-out-of-my-gourd frustrated with this and it has been going on for too long.

THANKS!

DAN

[MrWild]

If you're using servos, you can't lose steps. The drive would fault out with a following error. Are the cuts the exact same G-code, just with a deeper cut, or is the entire code different after the tool change? I ask because A program cn be made to offset with incremental commands.

An area I'd check is the motor to lead screw couplings for tightness. Paint a witness mark on the motor shaft, coupling, and lead screw and do some cuts.

And last, are you sure you have servos and not steppers? Which drives do you have in your controller? If you have steppers, you need to slow down your feeds and rapids as you are most likely losing steps.

[rvt]

Dan,

I would create your own GCODE for testing.

Something like



G0 X0 Y0
G0 X1000 Y1000
G0 X0 Y0
G0 X1000 Y1000
G0 X0 Y0
G0 X1000 Y1000
etc...
etc...

This would move the router from point 0,0 to 1000,1000.
Do this may be 10 times and see if it comes back to the same spot each time. You could even touch the wood to see if this works correctly.

it's hard to imagine what really happens. But a photo of the problem would help more then a 1000 words. This sounds more like slippage then backslash because backslash doesn't grow incrementally.

If it's backslash you would see a offset error that is always smaller or equal to the error you see, it will never grow.

So my advice is to make some simple G-COde program, HAND coded so you know exactly what it's going to do to root cauze the problem.

Adding backslash compensation in Mach3 would be your VERY VERY last resort and you onyl do this if you are sure it's a backslash problem and cannot be solved by changing mechanics

[louieatienza]

Get a compression spiral bit.... then you don't need to swap bits out... Maybe your table is sturdier in one axis and not another?

[ger21]

Cutting in two different directions could definitely cause the problem your seeing. CCW will tend to pull the bit into the part, and CW will pull it away from the part. You may also be seeing bit deflection. And and flex in the machine will be magnified by your dual direction method.

From my experience, cutting CCW (conventional cutting) will almost always yield better results in wood. The exception is usually in hardwood to avoid tearout.

AS was mentioned, if you have enough power, a compression bit is best and will avoid a tool change. If power is lacking, try making two passes with the compression, but the first pass need to be deep enough to prevent chipping. Bits known as mortise compression are ideal for this, as well as thinner materials. You can also rough cut slightly oversize using two passes, and them do a single full depth finish pass. Any of these methods with a compression bit will eliminate the tool change at least.

As for being 1/32" off in one direction, you should be able to fine tune that by adjusting the steps/unit in motor tuning.

[rvt]

Gerry,

I think we knows that CCW and CW cutting does create some offset between each other, and depending on the stiffness of the machine it is always in some range.
However, how would CCW and CW cutting explains 'offset grows incrementally' ?

I agree with the toolchange, if that can be avoided it's best...

Dan? Any pictures for us yet?

Ries

[ger21]

Originally Posted by rvt However, how would CCW and CW cutting explains 'offset grows incrementally' ?

It shouldn't. We need to see some pictures and get a bit more information.

If you make all 3 cuts with the same tool, in the same direction, do you still see the same issues?

[Phife]

If you have a dial gauge you can check to make sure that when you command mach3 to move 1 inch it acutally moves 1.000 inch. Sometimes your steps setting could be off a little so instead of moving 1.000 inch it moves 0.998 or something.. like that.

There is a calibration setting in mach3 for this.

Check all your axis to make sure it is indeed moving 1.000" and not more or less

[louieatienza]

Just thought of this, since I remembered having a similar problem (though not as large as 1/32) on my machine. I had to tune up my y-z axes so that the z axis moves exactly perpendicular to the table...

[Sjotime]

Hello all!

Thanks for your thoughts. I had to leave this problem for a while and go make/spend some money.

I will try running everything counter clockwise from here on out. I like the compression bit suggestion as well and where I can I always try to use them. The offset precut makes sense too.

I have removed the belt drives from my machine and replaced them with 10:1 gear boxes: not cheap! but 0 backlash. And I still have the problem!

I think it is either bit deflection or an issue with flex in my Z axis which I am in the process of replacing. Eventually the entire table will be rebuilt at this rate.

The latest observations:
A square: ie cut using only one motor to move the router per side: Dead on.
A diamond: a square turned 45 so each edge requires both motors: two parallel edges are short by a 32nd, the other edge shows a step indicating that the final up pass runs long a 32nd.
A circle: shows the same overlap/short issue as the diamond. In addition it has flat spot in the Y direction, like the switch from heading out to heading in is delayed. Just typing this made me realize that indicates a drag or delay in the Y.

Other information: Step counts and gear mesh
I have been working with step counts in the Motor Tuning configuration in Mach3. In order to get to the above results I have very laboriously worked through a series of movements with a square and ruler such that each axis is dead on back and forth over about 18 inches. ** The challenge here is that the number of steps needed to move the same amount are very slightly different in each axis.** I've also worked hard getting the gear meshes tight so there is no slop in the mesh between the drive gear and gear track on each axis. I believe they are tight.

I will run some tests cutting all in the same direction. The diagonal/curved cut issue is really irritating, but if I get rid of bit deflection, maybe the difference in steps/in setting can be eliminated. I wonder if I am compensating for bit deflection by motor tuning... But when I test for steps/in (motor tuning) I am not cutting.

Ah the joys!

So happy you guys jumped on this and sorry for disappearing. I appreciate all your input.

Dan

[hemsworthlad]

Make a pen holder and use a really fine ball point pen lightly touching paper then test again this will show better how much stepover there is and pritty much eliminate cutter deflection.

In your initial post you mention servo's but did you mean servo's or steppers.?
Can you give more detailed info on full machine details.! . . . Inc computer spec.

It will be far easier to help if we know the exact componets used, make model numbers etc of electrical components inc PSU spec (Volts & Amps) also If servo's encoder count.

Would help if gave a general discription of mechanical components used on machine with any info you have on pitch or pulley ratio's etc, Also good quality pics from various angles of important area's like Z axis and motor connections help considerably.

Give setting used in Mach motor tuning. . . . Edit: Inc the step/dir pulse timing settings just to the right of Acceleration settings

If the build quality is resonably good then I wouldn't go changing major expensive area's like the Z axis because it will more than probably turn out to be something electrical, whether that be noise, computer pp probs or dodgy wiring who know's yet but quite sure it wont be mechanical because of the repeatabilty, Yes mechanical would cause it but it would also be obvious and quite easy to find and I presume you have done the obvious like tightening motor connections and backlash checks.? (If not do it before you do anything else)

Give this info and i'm sure well all help track it down quicker.

Dean.

[Sjotime]

Dean,

Thanks for your response and indeed all that information is important to know for a decent evaluation. I don't have all that in front of me at the moment, but the current status is:

I replaced a goofy belt drive set up with 10:1 gear box and THAT has a bunch of slop in it, despite it's stats saying .002 backlash.

More like .020 accumulating to .040 forward and back plus the other axis. Can't cut a six inch diamond without distortion such that face to face they don't match. Can't cut a circle without a 1" flat spot on each side because of the slop in the Y axis. Am I asking too much here?

I'll get that stuff over the weekend and pass it on. Perhaps some insights will occur. Personally I'd like to have it so I can find out what the components are worth on eBay. I am seriously considering getting rid of this thing.

Thanks for taking the time and I will post as much of the info you noted in a few days.

Dan

PS: What I know off the top of my head:
>10000 DC Aerotech Servo Part# 1135-01-1000-99
>US Digital (?) 1000 line optical encoders
>Gecko Drives (no details in my head)
>Just replaced the cables with new ones that have little drivers at the encoder/motor end
>Rhino to Visual Mill to Mach 3 GCODE/Controller software workflow
>5' x 10' bed
>Transmission: Motor to 10:1 reduction gear box to spider coupler to drive shaft to drive gear meshed to toothed track
>Steps per in Motor Tuning are different per axis based on measuring travel vs DRO. Around 450.
>Don't know acceleration etc. I've always thought the motors weren't "strong" enough.
>Note: There is not feedback from the motor to the computer: You can grab the axis, push on it, move it (past the slop), see the motor shaft move and bounce back and no change registers in Mach. Should it?

THANKS!