Need Help!- Jerking

[TURNER]

Hi guys,
Could anyone give me any pointers please. We have a 2000 VF4 haas mill which has been running fine from new, recently we have tried some new highspeed toolpaths from a cam system. The machine couldnt hack it and was jerking. Is there any settings that could be altered to maybe help this. Please note we were cutting at F2000. mm/min and had to slow down to about F800. to get a smooth movement. We do not have the highspeed option. Also we have an older machine a 1994 model that we run some test pieces on before putting the live job on the newer machine and this run fine at F2000. and didnt start jerking till around F2300. I have also seen there is a setting 85 was set at 0.127 tried making that smaller and bigger with no noticeable effect.
Any advice greatly appreciated.
Thanks,
Keith.

[ToyMaker94566]

What kind of cut are you performing, are you 2D profiling or are you 3D surfacing? Are you running short little line segments or are you cutting G2 G3 arcs?

[WallyL7]

First off...CHANGE THE TITLE, MAN! For goodness sakes.


Well first of all, you are on track with setting 85. I think it comes from haas at .02"...so try that instead of your .005" - It will change the jerky-ness of the machine.



Next, make sure that the surface (right by setting 85) isn't on "finish". Put it on "medium".

And last - but actually first - make sure your filters are on big time on your cam. Mastercam has some great filters that make all those little moves much smoother arcs so that slow, old equipment can handle it better...

Other than that, you'll only be able to get away with so much. The VF-4 is a clunky type machine with a fairly heavy table. Those tiny moves with a large table just punish a fairly weak machine like Haas.

[TURNER]

Originally Posted by ToyMaker94566 What kind of cut are you performing, are you 2D profiling or are you 3D surfacing? Are you running short little line segments or are you cutting G2 G3 arcs?

Hi ToyMaker, it is mainly 2d arcs / lines, some segments are quite small. There is some 3d shortline segments that produce a helix entry to Z-depth.
Keith.

[TURNER]

Originally Posted by WallyL7 First off...CHANGE THE TITLE, MAN! For goodness sakes. Well first of all, you are on track with setting 85. I think it comes from haas at .02"...so try that instead of your .005" - It will change the jerky-ness of the machine. Next, make sure that the surface (right by setting 85) isn't on "finish". Put it on "medium". And last - but actually first - make sure your filters are on big time on your cam. Mastercam has some great filters that make all those little moves much smoother arcs so that slow, old equipment can handle it better... Other than that, you'll only be able to get away with so much. The VF-4 is a clunky type machine with a fairly heavy table. Those tiny moves with a large table just punish a fairly weak machine like Haas.

Hi Tim, lol (title), reading it back. Anyhow thanks for your input, so i make the setting 85 larger yes? and i didnt notice the other medium/ finish thing so ill take a look tomorrow. You also mention the VF4 being naturally Clunky, this has not showed up before as we have only done pretty simple operations on it. Saying that i have been told there will be some investment into replacing 2 of them maybe this year or next. Do haas do a better alternative machine?, i know they are cheap, but if they are not up to the new tech we may be better looking at alternatives.
Keith.

[Wizzard of H]

Since you do not have HSM and you said this is only XYZ motion, there are only two causes for this.

1) The first is just short strokes. If the stroke length is so short that the control cannot accelerate up to speed and decelerate down to stopped in the length of the stroke, you will not get up to speed and it will appear to start and stop at each stroke.

2) The second cause is how each stroke blends with the next. If they are nearly in line, the control will overlap the deceleration of one stroke with the acceleration of the next and the speed could be near as programmed. If they are sharper angles, the control will be forced to slow down to meet the setting 85 criteria. A 2000 machine will not have Rough, Medium, Finish setting 191.

Finally, if you can't solve with 1 or 2 above, you may need HSM which can be purchased even now.

If still stuck, post a piece of the G-code along with feed rates.

[ToyMaker94566]

Originally Posted by TURNER Hi ToyMaker, it is mainly 2d arcs / lines, some segments are quite small. There is some 3d shortline segments that produce a helix entry to Z-depth. Keith.

Does the machine thump on the short lines or just on the arcs or both?

Also, who makes your CAM system. I would start with your CAM system to solve the issue. As mentioned, your posting filters can make all the difference in the world. I will also say, most thumping issues have more to do with arc interpolation when high speed machining. The older processors need help from your CAM to smooth your passes. I would avoid small arcing code, G2 G3... and opt for line segments but without a high speed machining processor, that too has its issues.

[WallyL7]

What are the rapids on that machine? I remember we had a 1200(I think) rapid Haas - one of the first after the typical 710 machines - and it completely sucked on anything intricate - and it was a VF-2!!

It actually couldn't do these little medical parts that I was running previously on an old VF-2 with 710 and .015" endmills in stainless. It was just too jerky.

You are right about increasing the number on setting 85. It will allow a bit of sloppyness - if you will, so you may or may not be able to get away with just opening up that number.

By clunky-ness - outside what I said about the 1200 ipm machines - again, the VF-4 is a pretty good size machine with a pretty heavy table and Haas uses pretty weak components, and without HSM, you are just going to get what you get.


Play with those numbers - if your tolerance is way open, try making the "surface" to "rough" even...and perhaps even a larger number on setting 85. You can also just program a G187 to change setting 85 and the surface for specific sections of code, then have it change back for finish passes.


Wizzard - I didn't remember that those machines didn't have the surface designation. Disregard that suggestion.

[SBC Cycle]

There are a few threads about this subject and I didn't want to dig up an old one so...

I'm trying to wrap my head around why my VF3s are so jerky. The short line segments I somewhat understand (not really but I'll get back to that). What really puzzles me is why the control slows down for arc segments ie. G2 and G3. It doesn't matter if it is an inside arc or outside, it slows to probably 70-80 percent of the programmed feed rate. EDIT: Actually it doesn't slow down as much on outside radii but is probably more like 50 percent feed on inside radii.

CUTTER COMPENSATION:
Yes (G41)

TOOL:
0.5000" 3F

MATL:
Acetal (Delrin)

FEED:
70 IPM (Extremely conservative, yes?)

SMALLEST INSIDE RADIUS:
0.3906"

LARGEST INSIDE RADIUS:
0.5075"

I tried turning on the HSM feature for a load of parts and it smoothed out the tiny line segments but didn't help with arcs slowing down. I'm very surprised that my box way Fadals can handle the tiny line segments and arcs at speeds in excess of 230 IPM without slowing down (and infinitely smoother) but the Haas can't.

Other than this not so small problem, these have been fantastic machines. I'm hoping there is a setting I have over looked somewhere.

[Wizzard of H]

The effect you are seeing is almost certainly something done with cutter compensation to insure that the "cutting edge" of the tool is actually running at the programmed feed rate. This only occurs when cutter compenation moves your cutter to the inside of a curve. The minimum reduction in speed is usually 50% and is specified by setting 44. This is a feature that has been part of Fanuc and other controls for close to 20 years. If you don't want it to occur, put a value of 100 in setting 44.

[SBC Cycle]

Originally Posted by Wizzard of H The effect you are seeing is almost certainly something done with cutter compensation to insure that the "cutting edge" of the tool is actually running at the programmed feed rate. This only occurs when cutter compenation moves your cutter to the inside of a curve. The minimum reduction in speed is usually 50% and is specified by setting 44. This is a feature that has been part of Fanuc and other controls for close to 20 years. If you don't want it to occur, put a value of 100 in setting 44.

That is exactly what I suspected, I knew there was something I was missing. The Haas has been proving itself to be very well thought out. That's a neat feature that I will probably use a lot. Not this time, but in the future for sure

Thank you very much.

If I can ask one more question, is this a simple feed rate reduction percentage or is there a tool radius / corner radius correlation?

[Wizzard of H]

Is's a function of the radius change caused by cutter compensation.
If the tool center path goes thru a radius half of what is programmed, the feed rate will also be one half. So, program a radius of 0.75 inches with a 0.75 diameter tool (0.375 radius) and the tool path will have a radius of 0.375 inch.