Roland RML Post processors

[Anonymous]

Hi HSMWorks
At Roland we have our traditional RML (Roland machine Language) that works on all machines.  Then with some newer models we have ISO G-code, which your included Roland post works.  There are a lot of potential users who only have RML.  We have sold over 80,000 machines.

The current range of machines, MDX40A, MDX540, iModela use the ISO g-code or RML (0.01mm), the MDX15 and MDX20 only use RML (0.025mm).

RML is in 2 units. 0.025mm and 0.01mm, so there would be 2 posts required.

All moves are linear so circles, peck drilling etc has to be linear moves in Absolute, with all 3 axis repeated on every line as they are non-modal positions and no decimal points.

Basically if every move is output as 3 axis moves and the feedrate is changed from a rapid feed, Z feed and XY feed, the program works.

Assume the following on the MDX15/20 in this sample:-
Max feed 15mm/sec
Z feed 2m/sec
XY feed 7mm/sec
Z0 top of work
Intial clearance 10mm
Rapid plane 2mm
cut depth -0.5mm
No comments valid
; is EOB followed by a CR/LF


;;^IN;
!MC1;
^PR;
V15.0;                Max feed (G00)
Z0,0,16260;            Z=linear 3 axis move to machine MAX Z in G91
^PA;                  This line and above is fixe header PA=G90, PR=G91, !MDC1=M03
V15.0                G00
Z0,0,400;            X0 Y0 Z10.0
V15.0;                G00
Z0,0,80;              X0 Y0 Z2.0  (Rapid plane
V3.0;                Plunge feed (G01 F)
Z0,0,-20;            Move to X0 Y0 Z-0.5
V7.0;                XY Feed
Z400,0,-20;          G1 X10. Y0 Z-0.5
Z400,800,-20;        G1 X10. Y20. Z-0.5
Z0,800,-20;          G1 X0. Y20.0 Z-0.5
V15.0;                G00
Z0,800,80;            X0. Y20.0 Z2.0 (rapid plane)
!MC0;                M05  - This is the footer
^PR;                  G91
V15.0;                G00
Z0,0,16260;          Move X0Y0 Z max
^IN;                  End

I have attached a sample sheet.

If your interested, it could open up the world for more compatibility with Roland machines.

Best regards

Patrick

[AchimN]

Hi Patrick,

we will investigate that and come back to you ASAP.

[Anonymous]

Thanks Jr
If it is easy, then it could offer more potential business for you, us as well I hope.
Regards
Patrick

[Anonymous]

Is there already a post available for the Roland MDX40A? We are purchasing this machine and definitely need a post processor for it.

I found a roland iso.cps inside my HSM folder, would this be the post to use?

[fonsecr]

Yes, we have support for this CNC.

The post team can provide the post once you are ready to test it.

[AchimN]

Please try these two posts attached. One is for ISO format, the other one is generating the output in RML format.
Note that you have to set your machine type into the properties to get the right output for your machine model.

Special thanks to Patrick who helped us developing these posts!

[Anonymous]

I am using this roland rml.cps to generate script for a Roland MDX-40A.  I am having some trouble with the fact that I have a WCS origin different than the model origin. When I simulate the toolpaths, they look fine, but when I run them they seem to be doing something off in that they are not milling where they should.  I had no problems when the WCS origin matched the model origin.

[AchimN]

That sounds strange. Could you please send your part including your toolpathes to cam.posts@autodesk.com, we will have a look.

[lmlreg]

I just want to check if the roland rml.cps linked in this thread is the most current version of the post processor? My wife is trying to get Fusion 360 working with a Roland MDX-15 mill, and I want to make sure I get the right post for her.

[AchimN]

Yes those are the latest ones, make sure to set the property MDX15 to true during post processing to get the right output for your machine model.

[lmlreg]

Thanks so much  😄

[malinda_animegi]

Hi! Hoping someone has some tips here 🙂

I seem to be having a problem with the out put of the Roland post processor. Here's what I'm doing:

1) run a post on one of the paths I've created in the CAM section of 360
2) open the file in dropout
3) output the file to the machine from drop out

The machine moves the spindle to one position and then just sits running the spindle but not moving in the x or y axis.
(Attached File - 01.prn)

I ran a test with one of the models provided by Roland in dropout (using prn file exported from the modela software) and it seems to run just fine. (Attached File - Surfacing1)

Looking at the code in the 2 files, it seems that the code output from the post processor in Fusion 360 does not match up to the code output from the modela player software. The header and the last few lines of code are different and the y & z formatting doesn't match either.

Any ideas what the problem could be? I have the process selections for my machine set up as shown in the screen shot in the thread for my machine (MDX 15)

[lmlreg]

The problem is just that you have your starting coordinates in the wrong place. Since that Roland has no way to set zero work position, all X and Y moves need to be positive from the home position in the bottom left corner of the work envelope. The best procedure is to have a sketch of the work envelope in you part, and create the coordinate system from that sketch, to position your workpiece wherever you want it on the work table.

[AchimN]

Lee, thanks for sharing this!

[tonyt]

I have a mdx-40a hooked up on a win7 system running inventor 2016 w/HSM Express. I need to know how to get HSM to send the code to the MDX.
When I try to identify the machine in the post processor it only allows me to pick a com port, not a usb port – this machine is hooked up thru USB and there are no com ports on this computer.
I have actually seen the machine cutting using HSM express on YouTube and there are people on the forum who say the can do it but I can’t seem to find the info I need to get it to start working.
please help
thanks
tonyt

[kaptekarev]

tonyt@wv wrote:

I have a mdx-40a hooked up on a win7 system running inventor 2016 w/HSM Express. I need to know how to get HSM to send the code to the MDX. When I try to identify the machine in the post processor it only allows me to pick a com port, not a usb port – this machine is hooked up thru USB and there are no com ports on this computer. I have actually seen the machine cutting using HSM express on YouTube and there are people on the forum who say the can do it but I can’t seem to find the info I need to get it to start working. please help thanks tonyt

I'm having the same problem. Where you able to resolve this issue?

[Laurens-3DTechDraw]

I gave an answer here:
https://camforum.autodesk.com/index.php?topic=7829.msg36288#msg36288

[stelzz]

Is there already a post available for the Roland SRM-20? Definitely need a post processor for it. Thanks!

[kushlik]

Hi,

I just wanted to report a bug in the Roland MDX post processor (observed in HSMXpress_2018_ML_R3_42644_Win_64Bit_dlm.sfx.exe). The post processor works, but the spindle does not start up on MDX-540. There is an error in logic in roland rml.cps in onSection() function:

line: if (getMachineType() == "mdx-15/20") {

should be : if (getMachineType() != "mdx-15/20") {

(fix confirmed)

Regards,

Alex