Centroid CNC M400 support

Post by **oloynet** » Mon Jan 08, 2007 11:10 pm

Hi,

I want to know if the Centroid CNC M400 is supported on VCarve Pro ?
http://www.centroidcnc.com/
Otherwise, what is the equivalent processor can be used ?

Regards,
Olivier

Post by **BrianM** » Tue Jan 09, 2007 3:50 pm

Hi Olivier,

I don't think we currently have any customers with that control. I've had a look at the web-site and it mentions 'back-plotting' g-code but it is not very clear if it can just load g-code. I would try to see if it can load the output from either the standard 'G-Code' post processor or the 'Fanuc' post as these are pretty generic. If these don't work , please can you send us a sample file for the machine to support@vectric.com and we will take a look.

Regards

Brian

Post by **oloynet** » Sat Jan 20, 2007 12:00 am

It works now !

Thanks to Brian who help me to support now the Centroid M400 CNC with VCarve

Olivier

Post by **cnckeith** » Sat Apr 07, 2007 6:22 pm

Hello. fyi.. All CENTROID CNC servo based control systems use G code that is similar to fanuc om with a few exceptions. (comments and tool changes)
I see in the V carve software a CAMtech RMS post. This might already be a CENTROID post since CAMTECH had used CENTROID software for the RMS machine a few years ago. I created a simple g code program with the RMS post and it backplotted just fine with my offline CENTROID software.
If Vectric is interested I can be of assistance in supplying any information needed to create a official Vcarve CENTROID post. There are about 10,000 centroid cnc controls right now worldwide that use the same style of g code. Since 1991 the models are M4,M40,M50,M60,M10,M15,M39 and M400. so the one post would work for all. kudos to the v carve team for such a nice pc. of software.

Post by **cnckeith** » Mon Apr 09, 2007 4:16 am

I've played around some more this weekend and the "G code ATC Inch.tap" post has been working on my CENTROID equipped router. I made several Vcarve test cuts with no problems. I discovered, that the camtech post I mentioned in the last message does not support tool changes and is only available in mm. I'll post a list of all the supported CENTROID g codes for future reference. good luck with your projects..

Post by **cnckeith** » Sat Apr 14, 2007 4:06 pm

CENTROID G Code list and description of operation attached. This should help answer any questions on how the CENTROID CNC control reads g codes. Brain can you make an official CENTROID post for us with this information? If you need anything else just let me know.

Post by **oloynet** » Sat May 26, 2007 7:59 pm

Hi,

Here the two post processors files to support Centroid CNC M400 (inches and millimeters).
I've made a lot of tests with them and they are OK since start of year.

Olivier

Post by **Tony Mac** » Sat May 26, 2007 8:25 pm

Hi Oliver,

Thank you for writing and testing the Centroid postp's and they will be added to
the standard installations of all products.

Tony

Post by **cnckeith** » Sun May 27, 2007 12:28 am

Awesome...I'll start testing the new posts and report back! thanks.

Post by **cnckeith** » Wed Jul 04, 2007 3:28 am

fyi.. I have been using the new CENTROID inch post with VCarve 4.0. So far so good. Thanks for creating it!

misc comments for the vcarve team about the post.

-Block numbers are nice but not necessary for the CENTROID CNC control.
(CENTROID's own conversational does produce block numbers but only at the beginning of major events.)
the CENTROID control can run, search, graph, do everything without block numbers so no limitations if you don't use them. It does support them so no problem if you put them in..just an old throw back to days gone by..

-CENTROID G code is modal so its not necessary to reproduce the G1 (or any g code) on every subsequent like line.

- It would be real nice and probably save a few cutters if the Vcarve generated program would move to the Z- rapid plane at the first XY coordinates of a plunge/ramp Rather than X0Y0. Right now, the tool moves to Z+.787 at the beginning of the program at X0Y0. The next move to the plunge position can be disastrous if there is something in the way. (Some of these moves can be huge long moves on a big router! covering lots of real estate with potentially another jig or fixture in the way ) A safer move would be to position to the first XY plunge/ramp position with the Z axis at the home position,THEN rapid to the rapid plane (Z+.787 in this case) and then begin the plunge/ramp on move. Here is the current output...

N0200 ; Tool Length Compensation Cancel - Move to Z home
N0210 G49 H0 M25 (M25 moves to the machine Z axis HOME position defined by the control user in the control setup, most often its max Z+)
N0220 ; Absolute Positioning Mode - Rapid Positioning
N0230 G90 G0 X0.0000 Y0.0000
N0240 ; Start Tool Change
N0250 T1 M6
N0260 ; Spindle on CW
N0270 M3 S21000 F100
N0280 ; Pause for 2 seconds
N0290 G4 P2
N0300 ; Tool Length Compensation (+)
N0310 G43 G0 Z0.7874 H1
N0320 ; ---------------------------------------------
N0330 G0 X2.1082 Y9.5498 Z0.2362

If block N0310 was to read: N0310 G43 G0 X 2.1082 Y9.5498 Z0.7874 H1 It would have the desired result moving from XYO to the plunge position with Z at the home position.

- The post says Vcarve 3.1 when V4.0 created it.

- you probably gathered this.. The pause and wait for dwell time is created by the CENTROID conversational since it is geared toward a milling machine with flood coolant, this gives the flood time to get pumping thru the system before the cutter hits the metal. For most router folks this is just an annoying delay. I just read how to edit the PP in a forum post so I'll be changing mine to suit my needs. thanks for making them editable!

Post by **Tony Mac** » Wed Jul 04, 2007 9:43 am

Hi Keith,

Thanks for the feedback on the postp.

If you can let us have a copy of your modified postp
this can then be added to the default list.

Tony

Post by **BrianM** » Wed Jul 04, 2007 10:35 am

Hi Keith

- It would be real nice and probably save a few cutters if the Vcarve generated program would move to the Z- rapid plane at the first XY coordinates of a plunge/ramp Rather than X0Y0. Right now, the tool moves to Z+.787 at the beginning of the program at X0Y0

The first move position is NOT hard wired into the post. This is the 'Home Position' you set when you calculate toolpaths in VCarve Pro and can be changed by setting the home position in the 'Material Setup' dialog. You can also set the Rapid clearance gap height here.

Brian

Post by **cnckeith** » Wed Jul 04, 2007 2:10 pm

Brain,

Hello. thanks.. yes I've seen the material setup dialog. thats nice to be able to set that position, however it would be even nicer if in addition to being editable like it is now, it would default to the first XY plunge position in the program for the rapid move to Z home (in this case +.787 or whatever you have it set to). That way this "smart" default would work for 99% of the programs generated and I'd only have to modify the material setup screen XY position for 1% of the jobs where I didn't want the Z plunge move to be at the same position as the first XY coordinate for the first plunge/ramp into the material, rather than the other way around. A few other programs I've used work like this and its a nice little feature and would probably save some cutters for VCarve newbies (like me:-)) thanks for the super fast reply, you guys are on top of your game! fyi weekend project photos attached.