Line/Arc Filter Settings

[tiredtoolmaker]

Re: MX7

 

See attachment

 

The instructor of the Mastercam classes I've attended told us to always check the line/arc filter settings box and move the slider to 50% especially on older machines that have slower processors. I have always followed his advice and would like to set this setting as a default, if possible. I have a feeling I might get hammered for wanting to use this setting for every job regardless of the jobs tolerance specs. Please advise.

[Colin Gilchrist]

That's a perfectly acceptable default to have turned on. I would recommend making adjustments to the "total tolerance" when you switch between roughing and finishing, but there will always be settings you should manipulate on an individual basis for a given path.

 

To set the defaults, do the following:

1. Outside of Mastercam (using Windows Explorer), navigate to your Shared Mcamx7 Folder. Go into Shared Mcamx7 > Mill > OPS. Inside that folder are the "Defaults" and "Operation" libraries.
2. Each of these "Default" and "Operations" files is really just a "Mastercam" file with a different file extension.
3. Rename the "Mill_Inch.defaults-7" file to "Mill_Inch.mcx-7". (Just change the extension. Press "Yes" when you get the rename warning...)
4. Go into Mastercam, and use File > Open, then browse to the OPS folder location.
5. Select the Mastercam file.
6. This opens the "Defaults" file as a normal MCX file. The file has an Operation for every Toolpath Operation type in Mastercam. Open each Toolpath individually and set your default values. This could just be modifying the Filter settings, or it could include any other "default" value you would like to be used every time you start a new Tool Path Operation of a given type.
7. After making your changes, save the Mastercam File, and completely exit Mastercam. (Probably not necessary, but do it anyway for safety's sake.)
8. In Windows Explorer, rename the "Mill_Inch.mcx-7" file. Change the extension back to ".defaults-7", and you've now got a modified Defaults file.

 

Now every time you start a new toolpath that references the "Defaults" file, it should come up with Filtering enabled, and set to your default values.

 

My only recommended change to your workflow would be to use 10-20% of your "Stock to leave" value for Roughing ops. So if you are leaving .03 on your Contour for Finishing, go ahead and use .003 for a "Total Tolerance" value. Then switch it to .0003 Total Tolerance for Finishing Operations. (Sometimes I'll use a Finish Tolerance of .0001 - .002. For Roughing, I'm typically at 10% of my stock to leave. So if I'm leaving .05 on my surfaces, my Total Tolerance for Roughing Ops would be .005).

 

Giving yourself "more tolerance" on a Roughing path will usually result in much shorter NC code, and tool path generation times that are shorter...

 

Hope that helps,

 

Colin

[tiredtoolmaker]

Thanks...works great!

[Colin Gilchrist]

[guitar]

That's a perfectly acceptable default to have turned on. I would recommend making adjustments to the "total tolerance" when you switch between roughing and finishing, but there will always be settings you should manipulate on an individual basis for a given path.

 

To set the defaults, do the following:

1. Outside of Mastercam (using Windows Explorer), navigate to your Shared Mcamx7 Folder. Go into Shared Mcamx7 > Mill > OPS. Inside that folder are the "Defaults" and "Operation" libraries.
2. Each of these "Default" and "Operations" files is really just a "Mastercam" file with a different file extension.
3. Rename the "Mill_Inch.defaults-7" file to "Mill_Inch.mcx-7". (Just change the extension. Press "Yes" when you get the rename warning...)
4. Go into Mastercam, and use File > Open, then browse to the OPS folder location.
5. Select the Mastercam file.
6. This opens the "Defaults" file as a normal MCX file. The file has an Operation for every Toolpath Operation type in Mastercam. Open each Toolpath individually and set your default values. This could just be modifying the Filter settings, or it could include any other "default" value you would like to be used every time you start a new Tool Path Operation of a given type.
7. After making your changes, save the Mastercam File, and completely exit Mastercam. (Probably not necessary, but do it anyway for safety's sake.)
8. In Windows Explorer, rename the "Mill_Inch.mcx-7" file. Change the extension back to ".defaults-7", and you've now got a modified Defaults file.

 

Now every time you start a new toolpath that references the "Defaults" file, it should come up with Filtering enabled, and set to your default values.

 

My only recommended change to your workflow would be to use 10-20% of your "Stock to leave" value for Roughing ops. So if you are leaving .03 on your Contour for Finishing, go ahead and use .003 for a "Total Tolerance" value. Then switch it to .0003 Total Tolerance for Finishing Operations. (Sometimes I'll use a Finish Tolerance of .0001 - .002. For Roughing, I'm typically at 10% of my stock to leave. So if I'm leaving .05 on my surfaces, my Total Tolerance for Roughing Ops would be .005).

 

Giving yourself "more tolerance" on a Roughing path will usually result in much shorter NC code, and tool path generation times that are shorter...

 

Hope that helps,

 

Colin

The only problem I see with this method is every time you update mastercam, mastercam will over write your defaults file since you chose to use the same name. Change the name (or folder) of the defaults file and update your configuration and machine definitions to prevent this from happening. Otherwise, good plan.

[Colin Gilchrist]

If you use the "Migration Wizard", it will take your existing files and carry them forward, using the Update process. No need to loose the work you put into customizing them. This will work for Tool Libraries, Default Files, and Operations files, even if you use the Default file names.

 

The only thing that will get screwed up when you Migrate it using the Migration Wizard, is the Control Definition Files, If and Only If, you don't take the time to set the "Control Definition Defaults". As long as you set the "Defaults" in the CD, then all your files can be carried forward using Migration, and you can certainly use the default file names.

 

If you plan to go this route, just install the next version of Mastercam, using the default installation. Then use the Migration Wizard to bring everything from your current version of Mastercam forward into the new version...