PDFThis document describes the setup of the machine, some of its dimensional limits, use of the Roland SRP Player software (for generating toolpaths from STL files), and some aspects of the process whereby an .RML NC file from MasterCAM is used. Harvard GSD (It could use some significant improvements.) Template File| View file |
|---|
| name | Guide to Roland MDX-40-A_2022.pdf |
|---|
|
Edit the NC FileThe .RML file that is generated by MasterCAM needs to be edited before it can be run on the Roland. Do this within MasterCAM's code editor or a text editor of your choosing. - Replace:
- the first line of the file, "!1", with "!MC 1"
- the last line of the file, "!0", with "!MC 0"
- Save the file with an extension of .RML (some text editors will save it with a .NC or a .TXT, which might have to be removed)
| Note |
|---|
Alternatively, replace the ROLAND MDX40 3 AXIS MILL INCH.PST file that is saved to C:\Users\Public\Documents\shared mcamx9\mill\Posts with the one that can be found on goliath: Z:\Software\Mastercam\Folder_Migrate_MCX_X9\put_contents_in_shared Mcamx9-mill-Posts |
Template FilesBelow is an empty MasterCAM template file files with a few toolpaths included within it (Rough Parallel, a few Finish Parallel options, and a 2D Contour toolpath)number of supported toolpaths included. The settings assume that 2" foam material is being used, so changes would be necessary for other material characteristics. Only one tool is Four tools are defined, so if using a different tool other than one included, a new tool will have to be defined. It is necessary that toolpaths using different tools be posted separately so that each tool can be have a new Z calibrated on the machine between toolpaths. Roland Template File | Note |
|---|
Presently (Fall 2016), the post for MasterCAM does not write out DRILL toolpaths correctly for the Roland Mill, so do not use these types of toolpaths. Contours and Surface-based toolpaths seem to be fine. Sales representative for MasterCAM has been contacted regarding the issue, but no solution was provided. For Drill toolpaths, the units are written in inches instead of being converted to millimeters (X,Y, and Z coordinates of drill points)| Info |
|---|
| icon | false |
|---|
| title | Recommended: Template File for Fanuc Machine Definition and Post Processor |
|---|
| Template Files on Sharepoint: Foam_Small_Roland_Mill This template file includes a Drill operation and is intended to be used with the Fanuc Machine Definition, Control, and Post Process (see below). |
Review the NC FileThere are two post-processors that you can select in MasterCAM to output an NC file for the Roland Mill, we recommend using the "Fanuc 3X Mill" machine definition as there are problems and limitations related to the Roland machine definition and post. | Info |
|---|
| icon | false |
|---|
| title | Recommended: Fanuc Machine Definition and Post Processor |
|---|
| The files that are most up-to-date can be found on the computer connected to the Roland Mill. The Fanuc 3 Axis Mill Machine Definition, Control, and Post Processor will output an .NC file. This .NC file should be reviewed for errors and needed corrections before it is run on the Roland Mill. Do this within MasterCAM's code editor. - Check for the correct Spindle Speed and Feedrate for the tool. This can be done by searching for M3 (spindle ON) and G1 (move with feedrate).
The speed is indicated by the Sxxxxx setting near the M3 (spindle ON/CW) command at the beginning of the program. The speed is given in RPM and the range is 4500-15000, for most tools and materials we will run near the top of the range. An example can be found on line number N130 with a G0, G90, G54 and then Z1.5 followed by the speed and spindle ON: N130G0G90G54Z1.5S15000M3 The feedrate for the Roland will vary from 30 IPM (inches per minute) to 120 IPM max. For low density foam, we can take light cuts at 70-90 IPM and G0 rapid/retract rates will be at the max of 120 IPM. The standard chipload charts are a reasonable place to start, but may have to be adjusted downward to meet the limitations of the machine. Look for the G1 commands and they will contain an F (feedrate) setting. An example here can be found at line number N160, with a G1 to Z.75 followed by a feedrate of 90 IPM: N160G1Z.75F90. - Check for Z0 and Z-, to prevent cutting into the machine table, this can be done by searching.
- Check for X- and Y-. This does not cause damage, but if G54 is set to the physical 0,0 (bottom left) then the machine will not move into negative territory. You can shift your model slightly and adjust stock on the table to compensate.
- Return to MasterCAM and make corrections there, if either of the above conditions need to be corrected.
Things to note: - In the VPanel, users must set the 0,0,0 of the "G54" coordinate system before cutting the RML file.
 Image Added
- The NC file does contain the spindle speed as defined in MasterCAM for the tool/toolpath.
- Coordinates are displayed in inches.
- Drilling operations are supported.
- When aborting a job the machine will NOT automatically retract to a safe location: make sure you manually lift the tool up above the stock before resuming or starting a new job, etc.
- Toolchanges are not supported by the Roland MDX-40A. MCX files that use multiple tools must output the toolpaths for different tools separately and re-calibrate a new Z for each toolchange.
|
|