Help with smoothing machine motion on Haas VF4-SS

[Pitka_Guru]

 

Hello everyone!

 

New to the forum and posting, so please bear with me. I've been using Mastercam since v7.1 so I know my way around it a bit. My experience is in 3D form dies and molds with a bit of aerospace work.

 

We are currently running X7 and are having some issues with machine motion from the posted G-code. We have a Haas VF4-ss with the hsm option. My Haas VM-2 would run 500ipm (accel and decel permitting) using CAM Tool and I never had these issues. 

 

We've tried a few different Surface high feed toolpaths, Core rough, Opticore and Opti area to see if we can get smooth motion. We've played with tons of settings. Corner rounding, arc filter tolerances, smoothing, arcs as line segments etc. We even changed the HMM kernel arc creation style. HMM kernel and a larger minimum arc size in the arc filter have made the most difference but it's not where it should be. 

 

Any idea's, suggestions or criticisms are welcome

 

The 408 dimension is mm

 

Thanks in advance

 

 

Pitka_Guru

[Brando]

hey man heres my settings for and optirest path, i believe this gives you the least amount of posted code as far as the line/arc to cut ratio ,increasing the total tolerance will reduce the amount of code as well  

[specv]

What are the issues you are having? The SS machines are not very accurate at all, especially at high speeds.

[BenK]

If you can share a file it would allow us to better help.

[Pitka_Guru]

Thanks guys, I'm atttaching the part we are cutting. The issue for us is machine motion. It look as though the machine is stuttering through certain areas of code and others where it is flying.

 

I've attached a copy of the code from a toolpath that looks better than anything we've tried. This was using core roughing and a programmed feed of the machine max. Ive tried it with the hass G187 P1 command which is the rough smoothness setting to keep higher feedrates.  

 

 

ONLINE SAMPLE.MCX-7

Best Motion yet.txt

 

If needed I can attach my Toolpaths and post processor.

 

Thanks again!

 

 

[BenK]

If needed I can attach my Toolpaths and post processor.

 

Thanks again!

Ya the toolpaths is what I will need to look at to help you out. I wanted to check out what filter settings you were using.

[Pitka_Guru]

Ok Benk,

 

Ive attached the file with my toolpath, I'm attaching our post as well. This program was run with mastercam addvanced configuration set to match the attrached image.

 

 

EMASTERCAM TP.MCX-7

 

Thanks

[Pitka_Guru]

dbl post

[Chris Rizzo]

 

the machine is stuttering through certain areas of code and others where it is flying.

Then it sounds like a machine issue. The code isn't going to change machine dynamics. Have you experimented with the machine corner rounding and accuracy settings? (I can't recall what the par #'s are).  That certainly controls code/motion.

[Pitka_Guru]

Then it sounds like a machine issue. The code isn't going to change machine dynamics. Have you experimented with the machine corner rounding and accuracy settings? (I can't recall what the par #'s are).  That certainly controls code/motion.

Hi Chris, I have played with G187 using P1, which is the rough setting. Default is P2 medium. I've even used G187 P1 Enn, where E changes the default corner rounding from .635mm to the value specified by E. I've run all my tests with and without P1 just to confirm the difference.

 

I've also run a raster tool path at a 30 degree angle on the part. That seems to run smoother consider I am moving in all 3 axes and there are no arcs output because of the angle. Adjusting some smoothing settings have improved the part since I started this thread.

 

 

My best settings for roughing have been

 

.1mm total tolerance (I'm leaving .5 stock)

create arcs in xy plane where min arc is 20 mm and max is 1000mm with one way filter on and use maximal tolerance for both

Smoothing settings set to minimize number of points and shift points randomly along tool path

 

I'll keep trying and maybe I'll visit the guys at inhouse to see if they have any ideas. Thanks for the help so far guys.

[specv]

I still say its a machine issue, we have an SS model and we can't feed over 100 ipm without significant loss in accuracy. In order to make the SS models faster all Haas really did was change the pitch on the ball screws, making small feed moves more jerky/less accurate at high speeds. If we bought another Haas it would definitely not be an SS.

[htm01]

I still say its a machine issue, we have an SS model and we can't feed over 100 ipm without significant loss in accuracy. In order to make the SS models faster all Haas really did was change the pitch on the ball screws, making small feed moves more jerky/less accurate at high speeds. If we bought another Haas it would definitely not be an SS.

true,but it starts at about 40 IPM, we traded our ss for the vm

[BenK]

Why do you have your minimum arch set so large? I would run that at .1-.5mm. Also Your cut tolerance is 90.25%, try changing that to 50%.

[The Cathedral]

In my experience, using "shift points randomly" and "minimize number of points" together has never been a very good combination, as they seem to cancel each other out. For me it always presents code that, on long smooth surfaces it will make only a few lines of code, but when you get into a corner or detailed feature the number of lines explode. Even with look ahead, it becomes a lot for the machine to parse all of a sudden. I've found I get the most consistent results when I use "fixed segment length" to keep the distance between points more consistent, and keep look ahead a more consistent distance in front of the actual position.

 

This is just my experience; your mileage may vary.

[Pitka_Guru]

Why do you have your minimum arch set so large? I would run that at .1-.5mm. Also Your cut tolerance is 90.25%, try changing that to 50%.

Hey Benk, Ive tried Brando's setting he posted earlier and it was very jerky motion. So I've set it this way because when the post outputs smaller arcs the machine stutters. After trying tons of tolerance variations the larger minimum arc runs the smoothest. It's strange because I can post a program with min arc set to .1 and when the machine reads a move of R6.5 it stutters. I'll take the same program and change min arc to 20 mm and post it. In the area where the R6.5 was, which is now some G1, moves the machine does not stutter through them, it looks smooth.

 

I'm going to get the Cam tool guys to run a rough and finish on this part to see if there is any difference. Is it possible the geometry of the part is affecting the tool path in a way where it makes moves that influence a smooth machine motion?

 

Cheers

[Glenn Bouman]

I checked your Arc/Filter Tolerance settings and you have the cut tolerance set looser (.09")  than the filter tolerance (.0047)

This will not give you effective arc filtering (I wish Mastercam would not default to this when you enable the arc filter option:(

 

Set the cut tolerance to 30% instead of 90% and you will get better results and a smaller toolpath file.

[Pitka_Guru]

Thanks Glenn, i will give that a go

SpecV and Htm1, I knew Haas changed the ball screws but I have never given it much thought. It is an interesting idea that due to the pitch, moves on a SS might never be as smooth as my old VM.

 

I'd think that with the new high speed tool paths and all the corner rounding option we should be able to overcome this issue, at least when roughing?

 

Thanks guys, I'll keep testing and let you know how it goes.

[BenK]

Hey Benk, Ive tried Brando's setting he posted earlier and it was very jerky motion. So I've set it this way because when the post outputs smaller arcs the machine stutters. After trying tons of tolerance variations the larger minimum arc runs the smoothest. It's strange because I can post a program with min arc set to .1 and when the machine reads a move of R6.5 it stutters. I'll take the same program and change min arc to 20 mm and post it. In the area where the R6.5 was, which is now some G1, moves the machine does not stutter through them, it looks smooth.

 

I'm going to get the Cam tool guys to run a rough and finish on this part to see if there is any difference. Is it possible the geometry of the part is affecting the tool path in a way where it makes moves that influence a smooth machine motion?

 

Cheer

 

Have you tried turning off the arc filter and setting the smooth settings to a fixed length. I don't use arcs in my 3D toolpaths but I'm running Makino highspeed machine centers. I don't know how that would work in your Haas, with what your describing it might be worth a shot.

[Pitka_Guru]

Have you tried turning off the arc filter and setting the smooth settings to a fixed length. I don't use arcs in my 3D toolpaths but I'm running Makino highspeed machine centers. I don't know how that would work in your Haas, with what your describing it might be worth a shot.

I've tried with no filtering or smoothing but it wasnt very good. I'll try the smoothing in the morning and hopefully CAM tool will get back to me Monday so I can test out their code. Im sure camtool wasnt arc filtering and my vm2 was flying so i think there has to be a setting in mcam or in the post that is giving me this problem.

 

Benk, what sort of tolerances do you think I should run for roughing? Thanks for the suggestion!

[Gary]

Yes, I want to know how the cam tool code runs on same machine/ same part. I am curious if its the machine or the fact you are used to the vm machine. 

[Pitka_Guru]

Glenn, have tried the setting you recommended and it was not as good as the settings I have attached. The two images are my best settings yet for roughing and then for finishing.

 

 

 

With these setting I can run full feed of 16510mm/min using G187 P1 but it is still jerky on the moves where it enters or exits the part. While it's in the cut its pretty good all things considered.  

 

The weird thing is that with the raster settings below and no arcs anywhere in the code the machine will do 15000mm/min in 3 axes. It is definitely slowing down in 2 areas where I have sharp surface geometry but that is expected. The surface finish is not great but that is not my goal in this endeavor.

 

 

I should have the camtool stuff on Tuesday, as Im in Australia so I need to wait for you all to catch up.

 

Cheers!

 

 

 

[Pitka_Guru]

Update.

 

I've tried the roughing from Cam tool. The movements were smoother in some area's mastercam wasn't but overall they were very close. Either I have forgotten what my machine used to move like or the SS models ball screw pitch is the problem. The machine is feeding at 16510mm/m (650ipm) with both programs so that's pretty good considering it's a Haas.

 

Hopefully I'll have time to try Cam tools 3d toolpath tomorrow. We are starting to do a lot of 3d surface machining so I can post some pics of the surface finish and feeds and speeds.

[The Chipmaker]

 

 

In my experience, using "shift points randomly" and "minimize number of points" together has never been a very good combination, as they seem to cancel each other out.

  @ Cathedral My reseller told me to use the those two in combination. I have  a Haas also, maybe that is why.