iModela processor

Discussion of post processors for various CNC machines

iModela processor

Postby alan_UK » Fri Dec 18, 2015 12:58 pm

Hi,
Just joined the forum.

I am trial testing meshcam with my Roland Imodela CNC mill, but am having problems with the post processing, the imodela will use either Rolands RML-1 or NC Code, have tried several of the NC code (.NC) listed drivers in meshcam, the unit moves except the spindle, so need some help.

Thanks
alan_UK
 
Posts: 10
Joined: Fri Dec 18, 2015 12:49 pm
Location: London, England

Re: iModela processor

Postby Randy » Fri Dec 18, 2015 6:28 pm

Hi alan_UK, and welcome to the forum. I found an iModela profile for pcb-gcode at http://www.mariolukas.de/download/imodela.pp and it looks like pretty standard gcode with M03 for spindle on and M05 for spindle off. But I see a lot of the MeshCAM posts are lacking the spindle commands.

I downloaded the iM-01 Master Guide and it looks like iModela runs single-tool programs because it doesn't mention an M06 toolchange gcode so I took that out. I added M03 and M05 commands. Give this a try. Name it something like iModela_MM_arcs.con and put it in the posts folder.

Code: Select all
; MeshCAM iModela config
; modified from Basic gcode-MMarcs.con
; 12/18/15      added M03 and M05 spindle commands, removed M06 toolchange command
;
DESCRIPTION = "iModela_MM_arcs(*.nc)"
FILE_EXTENSION = "nc"
UNITS = MM
;Feeds
FORMAT = [F|#|F|1.1]
;Moves
FORMAT = [X|#|X|1.4]
FORMAT = [Y|#|Y|1.4]
FORMAT = [Z|#|Z|1.4]
;
START = "%"
START = "(FILENAME: [FILENAME])"
; The following is a dummy tool to keep CutViewer from generating an error when G20 is called without a tool
START = "(TOOL/MILL,0.1,0.05,0.000,0)"
START = "G21 (mm units)"
START = "G17 (XY plane)"
START = "([CUTVIEWERSTOCK])"
;
TOOLCHANGE = "([CUTVIEWERTOOL])"
TOOLCHANGE = "M03"
;
RAPID_RATE_MOVE        = "G00[X][Y][Z]"
;
FIRST_FEED_RATE_MOVE   = "G01[X][Y][Z][F]"
FEED_RATE_MOVE         = "[X][Y][Z]"
;
FIRST_CW_ARC_MOVE = "G02[X][Y][I][J][F]"
CW_ARC_MOVE = "G02[X][Y][I][J]"
;
FIRST_CCW_ARC_MOVE = "G03[X][Y][I][J][F]"
CCW_ARC_MOVE = "G03[X][Y][I][J]"
;
END = "M05"
END = "M02 (END OF PROGRAM)"


Randy
All opinions in this post are mine alone. I am not a MeshCAM employee, I do not have a financial interest in MeshCAM, nor do I speak for MeshCAM. MeshCAM user since Beta 5 in 2003. viewtopic.php?f=11&t=15333 :ugeek:
Randy
 
Posts: 1812
Joined: Wed May 14, 2008 9:50 am
Location: North Texas, USA

Re: iModela processor

Postby alan_UK » Fri Dec 18, 2015 6:35 pm

Hi Randy,

Thanks for your help, how do a get into the posts folder

Alan
alan_UK
 
Posts: 10
Joined: Fri Dec 18, 2015 12:49 pm
Location: London, England

Re: iModela processor

Postby Randy » Fri Dec 18, 2015 7:03 pm

Alan, here is where it is on my Windows machine.

posts.png
posts.png (24.27 KiB) Viewed 1806 times


By the way, I edited the provisional post above by updating the embedded name. I realized it wasn't displaying properly in the MeshCAM drop down list.

Randy
All opinions in this post are mine alone. I am not a MeshCAM employee, I do not have a financial interest in MeshCAM, nor do I speak for MeshCAM. MeshCAM user since Beta 5 in 2003. viewtopic.php?f=11&t=15333 :ugeek:
Randy
 
Posts: 1812
Joined: Wed May 14, 2008 9:50 am
Location: North Texas, USA

Re: iModela processor

Postby alan_UK » Fri Dec 18, 2015 7:35 pm

Hi Randy,

Many thanks understand what I need to do, (working with the actual code is all new to me) will give it a try tomorrow and let you know the results.

You are correct the imodela does not have a tool change routine, but when using its normal CAM software 'Player 4', when you change a tool, it will stop working so tool can be changed, then you tell it to contiue.

Alan
alan_UK
 
Posts: 10
Joined: Fri Dec 18, 2015 12:49 pm
Location: London, England

Re: iModela processor

Postby alan_UK » Sun Dec 20, 2015 5:02 pm

Hi Randy,

Programme working fine and is listed OK in the Posts folder, but I have a problem, I selected a different tool for the 'Finish' section in meshcam, but the programme just went through to the finish without stopping, I have looked through the meshcam code file and can only see the first tool listed.

The test piece was cut very well, as it was my first test am very pleased so your Post code is working well, there is a couple of minor faults, but think this could be due to the cutter settings working for the 'Roughing' cutting.

Is it possible to have the code stop for a manuel tool change, or do I need to create a different tolpath file for each change of tool.
The imodela controller is very basic, without any visual references to toolpath code so I may have a problem restarting the code.

This may all be very basic but have never needed to work with the code directly.

Thanks,

Alan
alan_UK
 
Posts: 10
Joined: Fri Dec 18, 2015 12:49 pm
Location: London, England

Re: iModela processor

Postby Randy » Mon Dec 21, 2015 3:26 am

Alan, since the iModela does not support tool changes you will need to output the roughing and finishing toolpaths separately.

Set up the roughing and finishing toolpaths and calculate them all. When the Save Toolpath dialog box appears, uncheck all the finishing operations and save the toolpath, adding "rough" or such to the filename to distinguish it.

roughing.PNG
roughing.PNG (161.18 KiB) Viewed 1789 times

When the toolpath is done saving, the Save Toolpath dialog will still be present. Uncheck the roughing and check the finishing toolpaths. Save the new file, with "finish" or such added to the filename.

finishing.PNG
finishing.PNG (158.22 KiB) Viewed 1789 times

You will have two separate single-toolfiles, each with the appropriate setup lines. The only thing you will need to do between roughing and finishing is to reset the Z axis to accommodate the different toolbit length.

Randy
All opinions in this post are mine alone. I am not a MeshCAM employee, I do not have a financial interest in MeshCAM, nor do I speak for MeshCAM. MeshCAM user since Beta 5 in 2003. viewtopic.php?f=11&t=15333 :ugeek:
Randy
 
Posts: 1812
Joined: Wed May 14, 2008 9:50 am
Location: North Texas, USA

Re: iModela processor

Postby alan_UK » Mon Dec 21, 2015 12:20 pm

Randy,

Thanks for all the information, will be spending today trying it out.

I use collets on the tools to set the z length, and can change tools without any of the settings changing.

Because the imodela unit can be swung back on its base, it makes tool changing easy and can set the collets before I carry out any cutting.

I use cutters with a shaft dimeter of 3 mm.

Any one reading this and thinking of getting an iModela may think this wrong as the unit is normally supplied with a 2.35 mm spindle, but the UK importer changes the spindle to 3 mm.
It also means that I do not need to use the fan (fitted on the shaft).

Will let you know my results.

Alan
alan_UK
 
Posts: 10
Joined: Fri Dec 18, 2015 12:49 pm
Location: London, England

Re: iModela processor

Postby alan_UK » Mon Dec 21, 2015 3:22 pm

Oildrum02.jpg
Closer view to show size, scale 1:42
Oildrum02.jpg (711.62 KiB) Viewed 1782 times
Oildrum_01.jpg
First test with meshCAM and my iModela
Oildrum_01.jpg (961.19 KiB) Viewed 1782 times
Hi Randy,

Carried out test and am very pleased with the results, only used one cutter, but used two path files, as an initial process to check how the Controller would show the two files.

Alan
alan_UK
 
Posts: 10
Joined: Fri Dec 18, 2015 12:49 pm
Location: London, England


Return to Post Processors

cron