Total tolerance for Smoothing Settings

[MZA2492]

Is there ever a situation to set the total tolerance to .0001? See above png for our current settings... Problem is setting this to .0001 takes a long time to generate with the equal scallop toolpath in mastercam.

If we set this tolerance to .001, will it effectively achieve the same results? This is my guess

 

 

[cncappsjames]

Yeah, that is  going to take a bit longer to process. The tolerance is 999x tighter. It's not very often I set the tolerance that tight.

[Guest]

On 2/5/2020 at 9:10 PM, MZA2492 said:

. Problem is setting this to .0001 takes a long time to generate with the equal scallop toolpath in mastercam

I have heard high tolerances can cause problems, you could use your machsim verify and compare with tight tolerances to see the variance in both cases.

[cncappsjames]

In addition to what @peter~ said @MZA2492, you want to run tolerances as wide open as you can. As a general rule of thumb that has worked for me over the years;

• On 3+2 Contour, Pocket, 2D HST, etc... operations I'll either leave the default tolerance (.001") or 75% of the feature's tolerance if under .001". So if my pocket profile tolerance was .0008 then I would set my tolerance at .0006". 
• On 3+2 surface machining operations - roughing, I'll set to between .0025" and .005" depending on how much stock I'm leaving. I'v found any more (.006"+) than that and the motion on the machine becomes a little too abrupt for my liking.
• On 3+2 surface Machining Operations I'll either leave the default tolerance (.001") or 50% of the feature's tolerance if under .001".
• On rotary toolpaths (4+1 and 5-Axis) paths, tight tolerances can be your surface finish enemy. There are several settings that can affect quality, tolerance being only one. Generally, you want to keep these as open as possible. 

JM2CFWIW YMMV

[JoshC]

On 2/5/2020 at 9:10 PM, MZA2492 said:

Is there ever a situation to set the total tolerance to .0001? See above png for our current settings... Problem is setting this to .0001 takes a long time to generate with the equal scallop toolpath in mastercam.

If we set this tolerance to .001, will it effectively achieve the same results? This is my guess

 

 

why do you want .015" segments? that will be a very large program, i hope you have high speed look ahead and a great machine to run those small segments at any kind of decent feed rate. 

[Guest]

33 minutes ago, JoshC said:

why do you want .015" segments? that will be a very large program, i hope you have high speed look ahead and a great machine to run those small segments at any kind of decent feed rate. 

Hmmmmm is that a thing, maybe this is our problem at my work, I will need to look into that, our machines our slow af doing anything other than a straight line.Althoo, I am pretty sure its off by default.

[JoshC]

5 minutes ago, peter~ said:

Hmmmmm is that a thing, maybe this is our problem at my work, I will need to look into that, our machines our slow af doing anything other than a straight line.Althoo, I am pretty sure its off by default.

it depends on the machine, some controllers run linear code great, like one that comes to mind is the makino controllers but some controllers or machines don't leave great finishes with 3d toolpaths or sometimes dont hit the programmed feed rate with a lot of linear code, longer line segments typically produce better 3d finishes on many low end / mid range controllers.

[Guest]

We have fagor 8065 controllers on dms 3 axis routers.

[JB7280]

On 2/8/2020 at 2:58 PM, cncappsjames said:

In addition to what @peter~ said @MZA2492, you want to run tolerances as wide open as you can. As a general rule of thumb that has worked for me over the years;

• On 3+2 Contour, Pocket, 2D HST, etc... operations I'll either leave the default tolerance (.001") or 75% of the feature's tolerance if under .001". So if my pocket profile tolerance was .0008 then I would set my tolerance at .0006". 
• On 3+2 surface machining operations - roughing, I'll set to between .0025" and .005" depending on how much stock I'm leaving. I'v found any more (.006"+) than that and the motion on the machine becomes a little too abrupt for my liking.
• On 3+2 surface Machining Operations I'll either leave the default tolerance (.001") or 50% of the feature's tolerance if under .001".
• On rotary toolpaths (4+1 and 5-Axis) paths, tight tolerances can be your surface finish enemy. There are several settings that can affect quality, tolerance being only one. Generally, you want to keep these as open as possible. 

JM2CFWIW YMMV

James, I appreciate this post, and it's actually a sticky note on my computer now.  However could you briefly explain how the arc vs linear vs smoothing sliders affect the toolpath and/or your part?

[crazy^millman]

I never use the smooth settings. To be honest not sure what they are supposed to do.

Here is what helps says. I was cutting molds well before any of this was added and still don't like and think it is not useful, but that is just my opinion and I am the dumb one in the room.

[JB7280]

6 minutes ago, 5th Axis CGI said:

But that is just my opinion and I am the dumb one in the room.

Hardly!

I pay close attention when I see your posts on eMC.

[JParis]

I have found smoothing to be quite machine specific.

Many machines will simply run cleaners on arc filtering ans highspeed codes....there are machines that better run on point to point info even in highspeed mode...these machine alone, in my experience, are the best place for smoothing. Otherwise, I stick to arc filtering

JM2C YMMV