What causes tool marks in surfacing paths?

[bhayden10]

I am wondering if anyone can give me some ideas what would cause a 1997 Mazak 16a vertical mill to make tool marks like this picture? This seems to be happening everytime i try to run a surfacing pass on this machine. It looks like the tool dwells for a second and cuts deeper in that spot. We had the x and y axis rebuilt last year. It holds tolerances well but the finish is not good. I'm not sure if its the machine tool or if i'm not doing something on my surfacing passes that i should. I changed this pass to a 2d pocket with arcs on the ends and it does not gouge the part like before. I appreciate any input thats positive.

[MotorCityMinion]

  What tool path, and what tool? Tool path tolerance = ? Even the finish across the top of the part is kind of nasty. Quite a few possibilities here but  IMO, it looks like something is loose. Tool holders in the spindle or the machine itself. Put a indicator in the spindle, touch something in the Y axis, zero it out, then push /pull on the head, both directions and watch the indicator. Leave it set in Y and push /pull on the table. Repeat for X and Z as well.  Is the top of the part wavy, as in large scallops? Check spindle squareness as well. It looks like your cutter may not be perpendicular to the Z axis center line. 

[Scott Lundin Shopware Inc.]

Does your machine have linear guides or box ways with tapered gibs? I had a machine that created tool mark similar to your picture. The spindle head was tilting. Try the inicator mentioned in the above post to see if it is tilting. We tightened up the tapered gib and surface finish got better. I saw another case where the spindle was deflecting in the Z-axis. This was a brand new Mazak install. The spindle was not assembled correctly and they had to re-calculate the pre-load and re-grind the spacers.

[bhayden10]

Thanks for the reply, it was a surface high speed horizontal area toolpath. Used a .375 tool, both with a .05 radius and one with no radius. stepover was 65%. I don't do enough surface paths to get a good feel for the tolerance settings but this one was on "better" and cut tol was .00028 and smoothing tol was .0007. I just did the indicator test everything looked good except i could pull and push the spindle over about .001. Got me wondering so i checked our 414 and h400 and they both were about the same. My lead man said this is normal as long as they all come back to center? Seems odd to me. He checked the backlash and it had .001 in the x and y so we will adjust that. These are all old machines but we do take good care of them and not do alot of hard milling. Could it be that this old machine cant look ahead enough that it is actually pausing in places? I have seen it do this at times running over 60 ipm. but i was around 50 in this pass. Just not sure how these old mills handle these paths i guess and what settings should be used for these old controls. Thanks again for your input.

[micr0]

I am wondering if anyone can give me some ideas what would cause a 1997 Mazak 16a vertical mill to make tool marks like this picture? This seems to be happening everytime i try to run a surfacing pass on this machine. It looks like the tool dwells for a second and cuts deeper in that spot. We had the x and y axis rebuilt last year. It holds tolerances well but the finish is not good. I'm not sure if its the machine tool or if i'm not doing something on my surfacing passes that i should. I changed this pass to a 2d pocket with arcs on the ends and it does not gouge the part like before. I appreciate any input thats positive.

 

Is the machine actually dwelling at those spots? If so make sure that Mastercam isn't putting out a bunch of tiny moves that is causing the control to stutter or choke. I have run a 16A and 16B of that vintage (M plus control?) and the control and machine was fast enough do deal with most of the complex tool paths I threw at it. How are you holding the work piece? Those marks look like marks Ive gotten in thin pieces that weren't supported well or were warping. Is the surface coming out flat though rough?

[Mr. Wizzard]

All suggestions, so far, are good things to check out. I am wondering, however, if you checked through the code on the toolpath? Look for stock taken on last (finish) pass. If the spindle is deflecting on large amounts of material removal and sitting/changing direction/dropping .0005 or so on these spots, that could be the problem. When you get into the surfacing, there can be many things in the program that the machine will not like. It's not that there's anything particularly "wrong" with the machine. Sometimes, I've found that you just have to custom tailor certain surfacing programs to certain machines and see what they "like". Some like arcs programmed IJK, as opposed to R. Some would rather do heavy cuts in the Y-axis as opposed to the X-axis. Long story short, or I will ramble on forever, see if there's something in the program that you might be able to adjust to get the specific machine to be "happier" with it. Not that there definitely isn't something wrong with the machine. There could be. I just like to make sure I've double checked everything from a progamming standpoint, before getting into machine issues, cause that's a whole other issue. You can run in circles chasing down a machine problem.

Best of luck to you. Let us know how it works out and if you can solve the problem.

[Stan_z]

looks to me like a thin part and the tool might be suckin the part up. Also you may need to take a finish pass to improve the finish

[Brad Lisle]

What is your clamping method? Looks like material warpage at its best. Why such a small tool? looks like you could fit a 1" indexable in there. Try to minimize small movements. Also maybe add a M00 to unclamp/reclamp part with a lighter load. This may help allow the material to relax. To me it looks like the tool is pushing the material down and I'm assuming your finish pass is fairly light. As it goes around in the small areas material fights is way back up. Try to keep you toolpath flowing and as a few have already said minimize small movements will help. What is your depth of cut on your finish pass?

[bhayden10]

The part isn't so thin that warpage is my problem. I am holding onto the bottom lug in a vise its .375 thick. the outside wings are for clamping in the final op as this part does get thin. They get milled away. I have to use a .375 because it is .475 between the .05 tall square lugs. I am only taking .05 in the horizontal pass. My post is putting out I and J for radius's. I feel it may be that the control can't keep up with the code but we also have a haas that i try to use for most of my surfacing paths as it does a much better job so I haven't spent much time trying to figure out what these older Mazaks like or need to run good finishes in most cases. Thanks for the help guys.

[Newbeeee™]

We had a very similar thing happen when we initially started using lookahead (G05 / G08) on our fanooks.

If you look here at the piccy, this is what we were getting http://www.practicalmachinist.com/vb/cnc-machining/fanuc-oimc-hsm-g05-1-g08-158264/

 

Now, this was fanuc and you have mazak, but you did say that x + y axes were rebuilt.

So I wonder if they need servo tuning?

 

To solve our problem, it was 3x parameters (time constants).

http://www.practicalmachinist.com/vb/cnc-machining/fanuc-hsm-g08-g05-1-settings-171099/

 

If your machine has never worked well at feed, your parameters may never have been correctly set?

[MotorCityMinion]

 Cutting 58 to 62 rc  parts all the time with the horizontal path and I've never experienced those kind of results. Simple enough to check the code though. I've never seen the Z's change throughout a Horizontal tool path regardless of tolerance, on the same plane that is. Perhaps some jack screws under the part with rubber sandwiched between the jack and the part to help dampen the vibes some. 

[taperlength]

Like Stan sayz, the part is getting sucked up by the cutter. Take one or two light finish passes.

[Newbeeee™]

Brian,

Did you get anywhere with this?