Roland MDX-40A - wrapping postprocessor

Post questions, share ideas and techniques relating to 3D prototyping and milling
Post Reply
MorenoR
Member
Posts: 5
Joined: Wed Jun 24, 2020 11:03 am

Roland MDX-40A - wrapping postprocessor

Post by MorenoR » Wed Jun 24, 2020 11:42 am

Hello everyone,

Would anyone be able to tell me what configuration I should set Vectric Aspire v9.5 to in order to process files to cut rotary wrapped toolpath on the Roland MDX-40A? Is there a specific post processor I need to download?
I mean wrapped arround X-axis (Y=A) toolpath in mm.

I am attacing two "standart" wrap post processor configurations (from Vectric) for reference.

Many thanks.

Moreno R
WINCNC_WrapY2A_ATC_mm.zip
(1.09 KiB) Downloaded 14 times
WinPC-NC_ATC_RotaryA_mm .zip
(1.57 KiB) Downloaded 17 times

User avatar
Patrick Thorn
Gold Member
Posts: 334
Joined: Thu Aug 11, 2011 9:19 am
Location: Staines
Contact:

Re: Roland MDX-40A - wrapping postprocessor

Post by Patrick Thorn » Wed Jun 24, 2020 12:05 pm

Thanks for asking us.
Vectric would be able to help you with this.
https://support.vectric.com
Patrick Thorn
Premier Consultant - 3D Technology
Roland DG UK Ltd

http://www.rolanddg.co.uk

MorenoR
Member
Posts: 5
Joined: Wed Jun 24, 2020 11:03 am

Re: Roland MDX-40A - wrapping postprocessor

Post by MorenoR » Wed Jun 24, 2020 1:16 pm

Thank you very much, Patrick.
I will check with Vectric support team.

Have a nice day.
Moreno R

MorenoR
Member
Posts: 5
Joined: Wed Jun 24, 2020 11:03 am

Re: Roland MDX-40A - wrapping postprocessor

Post by MorenoR » Tue Sep 01, 2020 2:35 pm

Hi Patrick and all the others,

this is really difficult for me as a hobby user to output an appropriate workable NC code from my self-manipulated post processor for MDX-40A assembled with ZCL-40A Rotary Axis Unit.
I have study both NC Code Reference manual and Vectric post processor manual and I am still working to get the right settings in Vectric software.

I think I have managed the most of it but there are two things, I don't know, how to handle.

- As this is wrapped around X axis output and all Y values are output as A, there are NO Y moves output and the tool is assumed to be aligned with centerline of cylinder
- X Values are output as X
- Z Values are output as Z

- Machine settings is fixed to - Automatically (RML-1/NC code) and User Coordinate System. (Maybe I have to use Machine Coordinate or G54 -:-G59 workpiece coordinate)

- Output is generated in *.nc file

What is inexplicable for me is that:

- despite that there is output for Z axis, there are no moves in Z. (Initially I have set the tool at the center of rotation and then move it as up as possible for safety reason. Then in the start of the program, the tool goes down under the centerline and then goes up as much as possible with no any next movies at all).

- I think I cannot manipulate the feed rate as the feed rate is the speed of Rotary axis. How could I manipulate the speed of A axis rotation with NC code?

Here is a little part of NC code written for MDX-40A with Vectric and my self-manipulated post processor

Code: Select all

( Profile circle 1 )
( File created: Sunday August 30 2020 - 03:05 PM)
( Roland MDX-40A-Rotary - Cylinder Along X Axis, Tool along Z axis )
( Material Size)
( Cylinder Length = 80.000, Cylinder Dia = 31.000)
( Z Origin for Material  = Rotary Center Line)
( XY Origin for Job = Center)
( X Origin Position  = X:0.000)
( Home Position)
( X = X0.000 Z = Z55.500)
( Safe Z = Z22.500)
()
(Toolpaths used in this file:)
(Profile circle 1)
(Tools used in this file: )
(1 = End Mill {1 mm})
(|---------------------------------------)
(| Toolpath:- 'Profile circle 1'    )
(|---------------------------------------)
%
G90
G21
M03 S10000
G00 Z55.500
G00 X0.000 A0.000
G00 X0.000 Z22.500 A73.930
G00 X0.000 Z20.500 A73.930
G01 X0.000 Z15.500 A73.930 F2
G01 X-0.396 Z15.488 A73.916 F2
G01 X-0.793 Z15.476 A73.872 F2
G01 X-1.191 Z15.464 A73.799 F2
G01 X-1.589 Z15.452 A73.696 F2
G01 X-1.987 Z15.440 A73.564 F2
G01 X-2.384 Z15.428 A73.403 F2
G01 X-2.782 Z15.416 A73.211 F2
G01 X-3.178 Z15.404 A72.991 F2
G01 X-3.574 Z15.392 A72.740 F2
G01 X-3.968 Z15.380 A72.460 F2
G01 X-4.362 Z15.368 A72.151 F2
G01 X-4.753 Z15.356 A71.812 F2
G01 X-5.143 Z15.344 A71.444 F2
G01 X-5.530 Z15.332 A71.048 F2
G01 X-5.915 Z15.320 A70.623 F2
.......... ............. .............
G01 X3.686 Z12.500 A72.663 F6
G01 X3.310 Z12.500 A72.910 F6
G01 X2.936 Z12.500 A73.129 F6
G01 X2.562 Z12.500 A73.321 F6
G01 X2.190 Z12.500 A73.485 F6
G01 X1.820 Z12.500 A73.623 F6
G01 X1.452 Z12.500 A73.735 F6
G01 X1.085 Z12.500 A73.821 F6
G01 X0.721 Z12.500 A73.882 F6
G01 X0.359 Z12.500 A73.918 F6
G01 X0.000 Z12.500 A73.930 F6
G00 X0.000 Z22.500 A73.930
G00 Z55.500
G00 X0.000 A0.000
M05
M30
%
I have tried it in fresh air (without any material and tool) and I think for A axis the feed rate speed is the same no matter that the [F] is output as F6 or F320.

I think if I manage to solve this two points the output NC code will be workable :)

User avatar
Patrick Thorn
Gold Member
Posts: 334
Joined: Thu Aug 11, 2011 9:19 am
Location: Staines
Contact:

Re: Roland MDX-40A - wrapping postprocessor

Post by Patrick Thorn » Tue Sep 01, 2020 5:15 pm

For feeds say of 300 mm/min

F300.0

Yes A moves will always be slower than X moves.


If it was in RML code , then this is the equivalent G code moves we would do.

%
G90
G21
M03 S10000
G54 G00 Z55.500 (SET G54 X where you want 0, Y0 and Z0 with your tool first measured then set to Center of Roatation)
G00 Y300.0 (THIS MOVES AWAY TO ROTATE LARGE JOBS)
G00 A73.930 (ROTATE TO FIRST A)
G00 X0.000 Y0.000
G00 X0.000 Z22.500 (FIRST Z CLEARANCE)
......

G00 Z55.500
G00 Y-300.0 (THIS MOVES AWAY TO ROTATE LARGE JOBS)
G00 X0.000 A0.000
M05
M30
%

Hope this helps as it look slike you are nearly there.
Patrick Thorn
Premier Consultant - 3D Technology
Roland DG UK Ltd

http://www.rolanddg.co.uk

MorenoR
Member
Posts: 5
Joined: Wed Jun 24, 2020 11:03 am

Re: Roland MDX-40A - wrapping postprocessor

Post by MorenoR » Fri Sep 04, 2020 10:52 am

Hi Patrick,

This is great! :) Thank you a lot for your help!

I have tried the last modifications in fresh air and I think everything is working. Now I feel much more secure and could check with material and tool.
Only a few little changes to do, than everything should work smooth and fine.

These are the last modifications.

Code: Select all

%
G90
G21
G54
G00 Z55.500
G00 Y300.0
M03 S9000
G00 A73.930
G00 X0.000 Y0.000
G00 Z22.500
G01 Z14.900 F200.0
G01 X0.000 A73.930 F200.0
G01 X-0.359 A73.918 F300.0
G01 X-0.721 A73.882 F300.0
...........
G01 X0.000 A73.930 F300.0
G00 A73.930
G00 X0.000 Y0.000
G00 Z22.500
G00 Z55.500
G00 Y300.0
G00 X0.000
G00 A0.000
M05
M30
%
So, thank you again!
I am happy to improve myself in CNC machining.

Best regards, Nikolai

User avatar
Patrick Thorn
Gold Member
Posts: 334
Joined: Thu Aug 11, 2011 9:19 am
Location: Staines
Contact:

Re: Roland MDX-40A - wrapping postprocessor

Post by Patrick Thorn » Fri Sep 04, 2020 6:18 pm

Nikolai

Good job. Test with something soft like blue foam or even wit polystyrene.

Maybe share the Finished post processor here for other VCarvers.

Send me a copy. pthorn at RolandDG dot com

Nice if you a picture of a resultant milled part.

Best regards
Patrick Thorn
Premier Consultant - 3D Technology
Roland DG UK Ltd

http://www.rolanddg.co.uk

MorenoR
Member
Posts: 5
Joined: Wed Jun 24, 2020 11:03 am

Re: Roland MDX-40A - wrapping postprocessor

Post by MorenoR » Tue Sep 08, 2020 9:23 am

Hi Patrick,

Thank you for your opinion of my work.

Your help and the detailed check on Roland NC programming manual was the key for me.

I have made same major changes, as I need to test the post processor output from different king of toolpaths like profile toolpath, pocket toolpath, v-carve toolpath, etc.

Yesterday I tested it with some different tools on PU foam material piece and now I could say that my self-modified post processor is almost finished and works smooth and accurate.

I will send you some photos by email and one video to download and check.

I have one question for now.
As the post is set to output only in G54, I need to set the machine to G54 coordinate system and then set zero for all axis.
This is not so hard to be done, as it takes only a minute, but what it would be if I remove G54 from the NC code and set the machine to "User Coordinate System"?
Will it work correctly?

I will send also a copy of the final post processor to your email. Just to do a few little changes and test with material and tools again.

Have a nice day.

Best Regards,
Nikolai

Post Reply

Who is online

Users browsing this forum: No registered users and 1 guest