Arc Filter/Tolerance for Surface Finishing

[Frank Caudillo]

Hi everyone,

 

At my shop we do a lot of high speed surface finishing on aluminum parts and we're struggling with the arc filter/tolerance fields to get the smoothest possible toolpath. What I would like to know is what settings other programmers have found success with? Right now we've figured out kind of a sweet spot with our total tolerance at .0025", arc filtering on and the sliders biased between 5-50% cut tolerance, and the right slider all the way to "smoothing". Are we not using this properly? We understand arc filtering for 2D high speed toolpaths but the surface finish with paths like scallop, blend, etc. are what's giving us the most trouble. I've uploaded a screen cap of what our typical settings have looked like. If anyone could offer better insight as to how these settings affect surface toolpaths it would really help out a lot. Our local dealer and most Mastercam applications guys haven't been much help to us. Thanks in advance. 

 

[gcode]

There are many variables involved in getting good surface finishes

One of the biggest is the machine itself.. brand, age etc etc

[crazy^millman]

Hi everyone,

 

At my shop we do a lot of high speed surface finishing on aluminum parts and we're struggling with the arc filter/tolerance fields to get the smoothest possible toolpath. What I would like to know is what settings other programmers have found success with? Right now we've figured out kind of a sweet spot with our total tolerance at .0025", arc filtering on and the sliders biased between 5-50% cut tolerance, and the right slider all the way to "smoothing". Are we not using this properly? We understand arc filtering for 2D high speed toolpaths but the surface finish with paths like scallop, blend, etc. are what's giving us the most trouble. I've uploaded a screen cap of what our typical settings have looked like. If anyone could offer better insight as to how these settings affect surface toolpaths it would really help out a lot. Our local dealer and most Mastercam applications guys haven't been much help to us. Thanks in advance. 

 

Arc Filter-Tolerance Settings.jpg

 

That is heading the wrong way. You are losing quality going in that direction with the filter settings. I would run 50/50 and go from there.

 

Filter is not the same as it use to be. They broke the association of what defines an arc. Use to get 4 lines of code for a circle feature if you had break at quadrants. Would get one line of code on 3D surfaces if post was told do do full arc. Now that is not the case.

 

Want to test my conclusions? Create a Primitive Sphere and throw a flowline toolpath or HST toolpath on it. Post the code. Set the filter settings to the highest setting and arc settings. See how long it takes to process the toolpath. (Really insane amount of time) Post the code. 

 

Save the geometry to a level and use the real arcs from the back plot and close them. Now make a 3d Contour using those arc. Post the code. Compare the codes from all 3 and you will see what I am talking about how the filters in Mastercam are broken and have been broken for some time. The formula for an arc is the same as when it was created, yet I keep hearing how today's filtering is different than yesterdays. Really? Machines just don't respond the same as they did. Really? So if I want to cut a sphere on any modern machine it will handle 1 billion lines of code better than 300 lines of code that are arc moves? I would love to put that theory to the test on a 1900 imp 60k rpm machine and see what shapes comes out better. 

[jlw™]

I have also noticed you only get arcs of the path falls perfectly on a plane. This could also reduce code... a lot.

[Guest]

I have also noticed you only get arcs of the path falls perfectly on a plane. This could also reduce code... a lot.

 

That's correct...how could you otherwise get an arc if you are not on G17, G18 or G19 planes....

 

This is where G68 plane rotation can help on some machines in certain situtations

[Frank Caudillo]

I have also noticed you only get arcs of the path falls perfectly on a plane. This could also reduce code... a lot.

 

Yes, and I do this a lot with 2D high speed toolpaths to really simplify the code. 

 

There are many variables involved in getting good surface finishes

One of the biggest is the machine itself.. brand, age etc etc

 

They're all newer machines, Fanuc Robodrill that is only a few years old, newer Haas VF5, brand new Okuma horizontal, etc. 

 

That is heading the wrong way. You are losing quality going in that direction with the filter settings. I would run 50/50 and go from there.

 

Filter is not the same as it use to be. They broke the association of what defines an arc. Use to get 4 lines of code for a circle feature if you had break at quadrants. Would get one line of code on 3D surfaces if post was told do do full arc. Now that is not the case.

 

Want to test my conclusions? Create a Primitive Sphere and throw a flowline toolpath or HST toolpath on it. Post the code. Set the filter settings to the highest setting and arc settings. See how long it takes to process the toolpath. (Really insane amount of time) Post the code. 

 

Save the geometry to a level and use the real arcs from the back plot and close them. Now make a 3d Contour using those arc. Post the code. Compare the codes from all 3 and you will see what I am talking about how the filters in Mastercam are broken and have been broken for some time. The formula for an arc is the same as when it was created, yet I keep hearing how today's filtering is different than yesterdays. Really? Machines just don't respond the same as they did. Really? So if I want to cut a sphere on any modern machine it will handle 1 billion lines of code better than 300 lines of code that are arc moves? I would love to put that theory to the test on a 1900 imp 60k rpm machine and see what shapes comes out better. 

 

And this is probably where we don't completely understand the math going on in the background with the tolerance settings. We did end up getting some much smoother toolpaths going with 50/50 on the cut tolerance and arc filter/smoothing. We basically just adjusted the settings until the path became smoother than before. Some surfaces did better with 50/50 and other looked better with bias all the way to smoothing. The paths looked decent with the default .0005" tolerance and, by trial and error, we found .0025" to be a sweet spot. Is there a tolerance that you would recommend? The surfaces we're driving are all almost strictly cosmetic and, as such, we just need them to look as smooth as possible without insanely small stepovers. 

 

I hope I'm not missing your point, just trying to understand as much about this topic as possible from the more experienced users. You guys have a wealth of knowledge and experience and I'm just trying to understand as much as I can. Thanks again. 

[Guest]

Frank,

 

Not to be a smart aleck but I think you've already missed the point...

 

On those 3 machines, you're going to wind up using different settings to achieve similar finishes....

 

and no matter how much smoothing and filtering you do, sometimes, the only answer is a tight stepover

 

I find a 2:1 ratio for me works on most things......for me...I do get down to a .0002 filter value sometimes with a .0015/.003 stepover

 

Your work  maybe different

[Frank Caudillo]

Frank,

 

Not to be a smart aleck but I think you've already missed the point...

 

On those 3 machines, you're going to wind up using different settings to achieve similar finishes....

 

and no matter how much smoothing and filtering you do, sometimes, the only answer is a tight stepover

 

I understand that. I guess I wasn't sure how powerful the filter/smoothing settings were in Mastercam and maybe we just weren't using them to their full potential. I understand that there are limitations in each variable of the process (the software, the machine, etc.) but I didn't know if we were handicapping ourselves by not knowing how to best use those settings.

 

I appreciate the help and, after seeing your signature, I thought you'd appreciate knowing we machine AR and other gun components!

[Guest]

I understand that. I guess I wasn't sure how powerful the filter/smoothing settings were in Mastercam and maybe we just weren't using them to their full potential. I understand that there are limitations in each variable of the process (the software, the machine, etc.) but I didn't know if we were handicapping ourselves by not knowing how to best use those settings.

 

I appreciate the help and, after seeing your signature, I thought you'd appreciate knowing we machine AR and other gun components!

 

 

I used to sell them....now I make them, along with a ton of other stuff

 

You with AeroPrecision by chance?  I know there's a few out your way

[Frank Caudillo]

I used to sell them....now I make them, along with a ton of other stuff

 

You with AeroPrecision by chance?  I know there's a few out your way

 

Negative, I work for Mega Arms in Centralia. Started as a button pusher almost 6 years ago and ended up in programming.

[Guest]

Negative, I work for Mega Arms in Centralia. Started as a button pusher almost 6 years ago and ended up in programming.

 

Nice product out of Mega Arms

[Frank Caudillo]

Nice product out of Mega Arms

 

Thank you, that is what we strive for. 

[jlw™]

That's correct...how could you otherwise get an arc if you are not on G17, G18 or G19 planes....

 

This is where G68 plane rotation can help on some machines in certain situtations

 

 

I'm talking about perfectly on the plane.  I am referring to helical arcs about more than XY planes.  So that the arc can be X1.Y1.   I0.J0. to X-1.Y-1. will be output as segments no matter what.

[Mjölnir]

 Machines just don't respond the same as they did. Really? So if I want to cut a sphere on any modern machine it will handle 1 billion lines of code better than 300 lines of code that are arc moves? I would love to put that theory to the test on a 1900 imp 60k rpm machine and see what shapes comes out better. 

 

i'm using a 30000mm/min (programmable feed rate) 36K rpm machine with a heidenhain itnc530 control and it performs significantly better with linear code than it does with arcs. i don't use arc filtering at all and smoothing is always set to present arcs as line segments with a fixed segment length. 

 

so it really depends on the machine, control, and options available, yes?

[crazy^millman]

i'm using a 30000mm/min (programmable feed rate) 36K rpm machine with a heidenhain itnc530 control and it performs significantly better with linear code than it does with arcs. i don't use arc filtering at all and smoothing is always set to present arcs as line segments with a fixed segment length. 

 

so it really depends on the machine, control, and options available, yes?

 

Yes agreed. How many shops have that machine and that capability? Then it becomes the other part of the conversation. Like I said I would like to test it. Put the same code on a HAAS, or any Oi control machine and see what happens when you run one with arc moves and one with liner. 95% of the market is not high end so why change the process to only support 5% of what is out there?

[Frank Caudillo]

i'm using a 30000mm/min (programmable feed rate) 36K rpm machine with a heidenhain itnc530 control and it performs significantly better with linear code than it does with arcs. i don't use arc filtering at all and smoothing is always set to present arcs as line segments with a fixed segment length. 

 

so it really depends on the machine, control, and options available, yes?

 

This is the conclusion I have come to. We have many different makes of machines at our shop, mostly Fanuc controls, but we'll probably just have to experiment. A lot of parts had been programmed with Surfcam years ago and now that our newer parts are being programmed in Mastercam we're trying to get the most out the software. However, the machine will be ultimately what dictates what we can do. Thanks everyone for the input. 

[crazy^millman]

This is the conclusion I have come to. We have many different makes of machines at our shop, mostly Fanuc controls, but we'll probably just have to experiment. A lot of parts had been programmed with Surfcam years ago and now that our newer parts are being programmed in Mastercam we're trying to get the most out the software. However, the machine will be ultimately what dictates what we can do. Thanks everyone for the input. 

 

There is the best answer right there. See what works and don't be afraid to test things. To many people keep thinking one sizes fits all. Sorry, but it does not and what works on one machine can be a dog on another. Where experience comes in. Experience is not what I consider all that more intelligent it is having done enough of the wrong things to see you can always find a better way. Like I said in another thread as long as you are making good parts and the customer is happy and your company is making money then a lot of the conversations are just academic.

[BenK]

Best thing you can do is sit down with the machine programming manual and see what smoothing options it has and go from there. I spent a lot of time programming and running Makino's and the ones with the smoothing options worked better if I just gave them line segments. Don't be afraid to test and ask the machine tool supplier for input. Nothing beats testing in this area.

[Matthew Hajicek - Singularity]

I usually run .0004" total tolerance, 20% cut tolerance, line/arc filtering on for all axis', one way filtering, no smoothing.  .004" to .008" stepover with .050" to .125" ball endmills.  Haas VF-3SS 15KRPM, < 1 yr old.

[crazy^millman]

Here is what I was talking about with the Sphere. The .0001 tolerance and Filter setting applied OP4 took 13 minutes in my I-7 6920 8 cores with 64GB of RAM. Compare the code from all 5 and tell me for 95% of the machines out there which one will run better. Why such a difference when everything should be about equal?

 

https://www.dropbox.com/s/kcnzy1orfv0zbev/SPHERE%20TEST.ZIP?dl=0

[Frank Caudillo]

I usually run .0004" total tolerance, 20% cut tolerance, line/arc filtering on for all axis', one way filtering, no smoothing.  .004" to .008" stepover with .050" to .125" ball endmills.  Haas VF-3SS 15KRPM, < 1 yr old.

 

We have a Haas VF-5SS that we've been using for surface finishing parts. Do you use the control's smoothing settings at all? It's controlled by either the parameter setting (Setting 191) or the G187 P1, 2, or 3 in the program. We didn't notice much difference with it, I'm curious if anyone else has had success with it. 

 

Also, do you know if Haas has any high speed look ahead options for their controls?

[Matthew Hajicek - Singularity]

I use G187 P3 E.002 for final finishing.  Main thing it does AFAIK is slow down in corners for geometric accuracy.

[Frank Caudillo]

I use G187 P3 E.002 for final finishing.  Main thing it does AFAIK is slow down in corners for geometric accuracy.

 

That makes sense. Thanks. 

[Tymar]

I am seeing some weird stuff with 2017, I am doing a raster cut now and I am not getting the finish that I am after, and the crazy thing is, I know I can get really fine finishes. Just not sure whats up.

[Newbeeee™]

Best thing you can do is sit down with the machine programming manual and see what smoothing options it has and go from there. I spent a lot of time programming and running Makino's and the ones with the smoothing options worked better if I just gave them line segments. Don't be afraid to test and ask the machine tool supplier for input. Nothing beats testing in this area.

For the Robodrills (we used to have 2) - we ran everything in G05.1 mode. This was better than standard mode for finishes (and gave 10% cycle reduction).

For all our other machines (0iMC, 0iMD, 0iMF) again we run in G05.1 mode for everything (except drilling/tapping).

The machines run a different set of parameters/algorithm compared to standard mode, but you have to see if the OEM has configured it okay.