[dingo0722]

Our VF3 is doing some surfacing and it seems to be having trouble smoothly cutting the surface of a part. It has a stutter between each block of code, like it is stopping then starting each line. Is there some setting/parameter that I should look for to help smooth out the motion?

[Machineit]

Is this a brand new problem that you have never seen before? How long have you run the machine?

Mike

[WallyL7]

You can control the accuracy of the machine in the machine settings (or with G154). See the manual for the factory spec and make sure it isn't set too high (or small in this case). Setting it to .005" or under will cause the "exact stop" type of situation when surfacing.

Also, depending on your programming software, you can filter the toolpath and add arcs when it can and that will help the control process the information faster and the drives to be able to move smoother.:banana::wee:

[dingo0722]

currently setting 85 is set to 0.001. Should I increase this to 0.005?

I dont ever remember this happening before with this machine. So I am wondering if a setting was changed

[WallyL7]

I think it comes from Haas set to .020" and the finish set to "Medium"

[Matt@RFR]

Yeah, .001 is waaaay off. Default should be .025.

Try this in the heading of your program: G187 P2. E0.025. Those are the default settings and should get you going.

[CNC MI]

Setting 85 is currently shipping from the factory with a default of .050 Although this is called "max corner rounding" it is an algorithim and not a tolerance as many assume. Good luck.

[WallyL7]

Setting 85 is currently shipping from the factory with a default of .050 Although this is called "max corner rounding" it is an algorithim and not a tolerance as many assume. Good luck.

Agreed. My statement of it "controlling the accuracy" was mis-leading...which is why I called it the "exact stop" type of situation.(jerky motion vs smooth motion)


It will, however, tend to take shortcuts when given a large number though so in reality...it can cause accuracy issues. I have seen this with the older machines so I leave the number VERY small unless just roughing.

[Pondo]

It will, however, tend to take shortcuts when given a large number though so in reality...it can cause accuracy issues. I have seen this with the older machines so I leave the number VERY small unless just roughing.

+1 on that.
I used to machine plastics a lot. The limiting factor on how fast we could surface was the tolerance we set in setting 85 (or the G187 command value). Too high a value and we'd get inaccuracies or small gouging in the parts. Too tight and the machine would stutter like you describe. We had to find the right blend of setting 85 and the feedrate to get the results we needed.

I also assume you are running the program from in the controller's memory and not from DNC, a floppy, or a jump drive, right? If not, then you could be hampered from data starvation as the controller needs more code faster than the connection can deliver it. The symptoms are the same as yours. It has happened to me before when surfacing aluminum and plastic.

[Pondo]

One more note:
We had a couple VF-3's that would retain the values input in a G187 line for subsequent programs even though it's not supposed to be modal. For example, we would run a roughing program with a G187 E.025 line (no P value in older machines). If we ran a finishing program next, then we would have to make sure that there was a G187 E.002 line at the end of the program or we'd get crappy finishes. I ended up changing my post to put it in every footer.
Doesn't seem to be a problem on my 2007 machine though.

[KenFoulks]

Please make sure that High Speed Machining (Parameter 315:4) is turned on. Ensure your G187 values are correct and being used.

[MotoDave]

I am running into this same issue during both a 'HSM' roughing tool path (~100 ipm, lots of small moves) and also 3D surfacing at 80 and 120 ipm using a 1/2" ball end mill (7500 rpm spindle). I turned on parameter 315.4 (HSM) for my trial 200 hrs, and it definitely helped. I'm a bit disappointed though since I didn't think I'd need to worry about the HSM option until higher feed rates than I'm working with.

I am running the programs from a USB thumb drive, since I couldn't stomach Haas's upcharge for more than 1MB memory. I ran a small portion of the tool path from the controller and noticed no change in speed, so I don't think the transfer speed from the thumb drive is causing issues.

[extanker59]

I have had the same problems. I worked around it by the previous poster's ideas to play with the default smoothness/corner rounding settings. I ended up leaving them at the factory setting (.05 and medium) and changing my feeds and, more importantly, changing my toolpaths in my CAM system. Found that numerous settings in CAMWorks worked better than others. If you use CAMWorks, I can go into it deeper.

[double a-ron]

+1 on HSM

When I got the volumill module for GibbsCam I noticed the tool path output was a ton of small arc segments. As a result, the machine was real jerky and I didn't get to fully see the advantages of a dynamic tool path. I decided to get the HSM option turned on and that made all the difference. One program ended up going from 45 min to just over 30. All that time savings from eliminating those exact stops. Highly recommend.

[cadcam]

This is do to no High speed look ahead and when running these paths there are allot of small moves and when you start turning the feed over 60ipm you have the jerking and this the machine can not keep up with the small moves that fast. I have delt with this for 20 years. Haas will give 200 hrs for trying this option out on the control being the High Speed look ahead as stated by Ken Foulks from the outlet.

[extanker59]

I'm not convinced it is the HSM, cadcam. We have HSM and we can get that symptom with the wrong CAM toolpaths. Maybe dingo0722 can update us?

[cadcam]

well I can agree with path typs as how are you handling the transitions between surface cuts. What kind of speeds are you talking about. as I have easily ran the HMC and the VMC haas's at over 400ipm for many company's with no issues doing roughing and finishing.

So I would like to see if Dingo got his or her's situation taken care of.

[extanker59]

There are lots of settings in CAMWorks that affect this. zig-zag versus zig only for example. But that increases cycle time considerably. And, counter intuitive (if you ask me), setting it to line moves only, makes for smoother finish. More but unless you use the same CAM it's pretty useless.
The size of the part and tighter curves affect it also. We make small parts with tight small radii. 17-4ss and titanium mostly
Going over 80 ipm is a waste of time unless the part is bigger with larger sweeping curves.
400ipm. I'd like to see that. Can you post a sample program for a 1/8" ball endmill cutting a simple 1" slightly curved top with .06 radii on edges? If this is possible on our VM-2 or VF-2ss, I need to know.

[cadcam]

extanker59, give me a sample of waht you want. I figure you are using SW so I can take that file. and I am figuring you want to be cutting alum with this path.
I do understand your thoughts on the 17-4 or TI. I usually do not go over 120 or so in Ti matters on the shape and the cuts.

[extanker59]

I sent you an email with the SW part attachment to your website contact. Thanks for looking at it.