Wavy finish in pocket

[Tony35]

How bout a cropped image of the problem area?

 

+1

[gcode]

My guess is there is something wrong with a lead screw in the area of the machine's travel

If its not to much trouble try moving the setup a couple of inches in X and Y.

If the problem goes away, your machine needs some maintenance..

Another thing you could do is make a note of the machine coordinates in this area

and have the machine ball bar tested, making sure that area of the machine travel is checked

[McLaren]

Try running the finish pass in reverse to see if the problem moves to a X-Y- corner.

[Müřlıń®]

I can't remember how that machine goes together but it sounds like a mechanical problem to me.

[BenK]

We have tried this on two different machines both A66 and both cut the same.Once I can I'm going to try it on our newer A61 to see if it cuts any better.

[Guest]

UHH What? I have no clue what you are trying to say there!

 

TTIWWOP = This Thread Is Worthless Without Pictures

[Roger Peterson]

does the code have a G41 for the finish pass?

is there any comp distance being applied at the machine? (does your radius list have a value in it?)

 

 

1. if so try running it without cutter comp on.

 

2. try linearizing the arc via the post, or breaking the arc up into many short lines and see if that makes any difference.

 

3. try turning off the high speed look ahead.

 

all of these can cause issues, if they do not cure the problem I'd have to agree and say you have a backlash adj. issue, a ballscrew issue, or a bad bearing on one end of your X axis ballscrew.

[Newbeeee™]

I wondered if it was excessive backlash compensation in the machine parameters.

But OP tried it on 2x machines with exactly the same results.

So it has to be G41 or something stupid like that shurley???

Can you post the offesnding bit of the code?

[jeff]

I don't think that cutter comp has any cause to this, I have this problem on 2 different machines also, and have been chasing down the culprit for over 2 yrs.

Could tool harmonics have something to do with this?

[McLaren]

That's why I suggested trying a different number of flutes.

[mig]

Try to look G-code .

Some times there is problems there as example -/+ R code if you using this mode.

[BenK]

I tried a different endmill and different holders now also. Didn't get any better.

 

 

 

[BenK]

Here is an example of the code. I marked the problem areas.

 

 

 

 

 

 

N198G0G54X-.9488Y-.1445S10000M3

N199G43H1Z3.

 

 

 

N348G41D2X-.6522Y.7236

N349G3X-.7582Y.721Z.435I-.0516J-.0543

N350X-1.0026Y-.2989I.7582J-.721

N351X-.9727Y-.3212I.0299J.0089 F10.

N352G1X-.6299F25.

N353G3X-.6059Y-.31J.0312 F10.

N354G2X-.3959Y-.1328I.6059J-.505 F25. <----------

N355G3X-.3814Y-.098I-.0157J.027F10.

N356G2X0.Y.3938I.3814J.098 F25. <-----------

N357X.3814Y-.098J-.3938

N358G3X.3959Y-.1328I.0302J-.0078 F10.

N359G2X.6059Y-.31I-.3959J-.6822F25.

N360G3X.6299Y-.3212I.024J.02 F10.

N361G1X.9727 F25.

N362G3X1.0026Y-.2989J.0312 F10.

N363X.705Y.7731I-1.0026J.2989F25. <----------

[HT]

Did you try run them with M250.

[Newbeeee™]

NCPlot backplotted it ok....

You could run the geometry with the Z high so it's only cutting a minimum depth which will illiminate tool deflection etc, but it doesn't look like that.

I would do a backlash check with a DTI manually, to see if there is mechanical loss motion, but I don't think it's that either.

To me it looks more like parameters or servo set-up (drift)?

Does the machine contour accurately when it's cutting good (verified with cmm)? I don't mean positioning accuracy as in drilling, but contouring/moving?

Strange one this...

[CNCCookbook]

Are you climb milling?

 

Consider trying a conventional pass just to see if it helps. Climb milling tends to deflect the tool into the wall of the cut. Conventional tends to deflect along the toolpath.

 

There's a diagram showing these deflections on my tool deflection page here: http://www.cnccookbook.com/CCCNCMillFeedsSpeedsDeflect.htm

 

Cheers,

 

BW

[mig]

I tried a different endmill and different holders now also. Didn't get any better.

 

 

 

 

To me it looks like G-code problem.

I would try to chenge geometry first and elimunate arcs from the program by chenging setting in mastercam .

Just take a look if problem will come again .

[gcode]

To me it looks like G-code problem.

I would try to chenge geometry first and elimunate arcs from the program by chenging setting in mastercam .

Just take a look if problem will come again .

 

I think its a cutter comp problem.. as in small moves and large comp value

how much cutter comp have you got on this toolpath..

control comp or wear

have you tried it with D2 = 0 ?

have you tried posting this with computer comp ??

[mchin-pilot]

1-Machine tools have parameter for back lash compensation adjustment. Check? and you can tighten up the electronic setting.

 

2 cents......

 

 

2-If your machine tool has tolerance(nurbs control) , check if it is switched on and have the right values set for the kind of toolpath you are doing.

 

3 Dont feed too fast.

[K2csq7]

Here is an example of the code. I marked the problem areas.

 

In the code you posted all of the "problem" lines have a feedrate of 25.0 and the rest of the path looks like 10.0.

Why the feedrate changes?

 

 

As newbeeeeee said, raise the tool up so it only cuts like .050 deep or so, and run it ridiculously slow to eliminate tool deflection. Are you sure the control is keeping up with the tool (i.e. tool not "pausing" for a split second and flexing back into the material while the control catches up).

[BenK]

Keith, those feedrates are what I had to do just to get by so we could make the parts. It doesn't matter if my DOC is .05 or .5 it still looked the same. The problem area is a arc that is around 1.5" long. It only happens at the beginning of the path and not between lines.

 

I'm going to go run the code in our A61 this morning to see if it does it on that machine also.

[Joe788]

My vote is for switching comp to computer, and getting rid of all those feedrate changes.

[BenK]

My vote is for switching comp to computer, and getting rid of all those feedrate changes.

 

 

The feed rate changes is what made it a decent looking part.

 

I just ran it in our A61 at 100. ipm and the part looked good. It has to be something with our A66's

[Tony35]

might be arc tolerance parameters

[McLaren]

I still say backlash issue and try running the path in reverse. If it is backlash adjusting your compensation won't help at all. When climb cutting the endmill will still pull the table from one side of the screw to the other. Compensation just makes it overshoot when reversing direction.