Arc Filter/Tolerance Settings for 3D surface toolpaths?

[Jason @ CPM Industries]

Does anyone have filter settings for a Haas mold machine. We are cutting 3d molds out of aluminum and It seems like the tighter the tolerance the more jolting I get, when I loosen the tolerance it runs smooth but might not have the right dimensions. Attachment shows what I currently have.

 

Thank you.

[Machineguy]

Move your cut tolerence slider all the way to the right. Re post and see how the machine reacts. (move you "z" up 5" or whatever it takes to not hit the part)

I have time to play with a VM-3 on those settings. Much smoother, So far

I started at .010 total tolerance. Worked fine.

Changing to .005 total. I'll let you know

 

Machineguy

[Machineguy]

Total tol of .005, .002 worked. Cut tol slider all the way to the right.

This is what I'm testing.

Scallop finish. Part is a pully with 15 spokes. I'm cutting the top of the spokes, about 1/8 wide, at a 15 deg angle.

Stepover .005", 3/8 ball EM. 100 ipm.

second slider at 70%, 30%.

Machine runs smooth at all spoke angles.

Flipping the second slider and reposting. Runs smooth

 

Machineguy

[Jason @ CPM Industries]

I will give that a try. thanks Machineguy

[duckdogers]

we cut 3d molds all the time in aluminium, with sliders set all the way to right on our hass machines.We found that sometimes in dnc mode the machine would use up program faster than being sent which caused machine to wait for program.Found out is was baud rates not the same.WE also found that if feed rates to fast machine servos had hard time keeping up(not high speed machine).I think that when sliders are all the way to right it creates a much longer program for machine to keep up if feed rates to fast.

[Jason @ CPM Industries]

Thanks for the info mhopper. What do you keep your total tolerance at when you have the slides to the right? Also what do you have for some of your line/arc filter settings?

 

Thanks

[Redfire427]

A VM3 only has a 50 block look-ahead ( to the best of my memory ), so if you tighten the tolerance, the machine will eat up code faster than the machine can execute, which will cause jerky movement and decreased feedrates. Setting 85 ( tolerance control ) will also have an effect on the accuracy as well as performance. G187 allows you to adjust the tolerance within the nc program.

 

Carmen

[Delcandoit]

We've had some similar issues with older HAAS machines. One thing that helps was to have the majority of moves in 2 axis at a time and not 3 (X,Y - X,Z - not X,Y,Z). When the machine tried to process 3 axis it slowed the feed rates down to much lower than programmed.

 

A setting that I love is "One Way Filtering" This will combine any lines of code that follow the same linear path instead of splitting them into small segments. This can dramatically reduce program lengths depending on the part. "Minimize number of points" will try to figure out a way to create your toolpath while reducing the number of nodes that are very close to each other. This setting can reduce code as well.

 

I have played with creating arcs in XZ and YZ but I sometimes get tool comp on an arc instead of a line which causes an alarm at the control of course. You can post code with certain settings on and then post a different program with other settings and compare them using a file compare program (usually already in your NC editor) and see differences that way as well.

 

Please let us know what you find out.

[duckdogers]

I could not sent cad data but I attached a file with one operation which has the settings we use all the time that gives us the smooth finish we need on our molds.Keep in mind the more complicated the part the longer the program

[duckdogers]

sorry ,sent wrong file.This is right file, only thing that changed was stepover for a finish pass.

[Jason @ CPM Industries]

Thank you. I will try these out and let you know how it goes,

[Chris Bloedorn]

 

 

Turn off your arc filter and linearize arc in the advanced configuration

[Jason @ CPM Industries]

 

 

Turn off your arc filter and linearize arc in the advanced configuration

 

Would that do the opposite? I always thought you need more I, J, K movements for a smoother toolpath.

[htm01]

 

 

Turn off your arc filter and linearize arc in the advanced configuration

mine doesn't say "Mastercam X8"

[Chris Bloedorn]

 

Turn off arc filter specifically for Haas -- seems to work the best

[JOHNAKA]

it is all in the feed rate. haas cant take more than 120 ipm. depend on your machine setting,

[Jason @ CPM Industries]

 

Turn off arc filter specifically for Haas -- seems to work the best

 

 

Like this?

[Jason @ CPM Industries]

When I run with no arc filters and a tight cut tolerance my Haas runs very slow and jerky even though I have High Speed Machining. I must be missing something. Do I need to play with mastercam machine dynamics?.

[Jason @ CPM Industries]

OK. After reading through previous similar topics most people have arcs filters turned off and cut tolerances tight. (.0002) Smoothing is another topic but seems like most have it turned on. I'm thinking it has to do with Haas settings now. If anyone has any more input on this it would be very appreciated.

[JOHNAKA]

is your high speed machining enable in the haas control.

[Jason @ CPM Industries]

Yes it is. Thanks