901 PART LOCATOR while doing Vee Grooves

[Brent Riley]

Im running a Vee Groove program and getting a "Reposition the cut part into the G901 Locator"

It will cut the size out with the right cutter then stops, waiting for some code input of some sort.

Is this where I put an x and y location to resume and start vee cutting?

Stuck on this message : NOTE 901 PART LOCATOR NOT G902 Locator

[jason galbraith]

Sorry can't help, but mate you should see what I have to do to get V-groove doors :/ There must be a better way than how I go about it

[Daniel Vonderheide]

Brent,

Post your code so we can see where it is stopping. Every cad/cam software is different and puts out different code.

[Brent Riley]

[CLS]
[PRINT " Now that the Piece is cut to Size, Move away any offcuts."]
[PRINT " that will interfere with the following slatwall operations."]
[PRINT " "]
[PRINT "Reposition the cut part into the G901 Locator."]
[PRINT "**********NOTE 901 PART LOCATOR NOT G902 Locator*********."]
[PRINT "**********NOTE 901 PART LOCATOR NOT G902 Locator*********."]
[PRINT "**********NOTE 901 PART LOCATOR NOT G902 Locator*********."]
[PRINT "**********NOTE 901 PART LOCATOR NOT G902 Locator*********."]
[PRINT "**********NOTE 901 PART LOCATOR NOT G902 Locator*********."]
[PRINT "**********NOTE 901 PART LOCATOR NOT G902 Locator*********."]
[PRINT " "]
[WINDOW ON]
M00
<----------------------------------------------------------------------------------------------Stops here.

(__________________________________________________________)
(__________________ CUT GROOVES ___________________________)
(__________________________________________________________)

M80L50
SET ZSHIFT=MATERIAL_DZ+UWASTE
SET XSHIFT=0.000
SET YSHIFT=0.000
G901


IF [DADOTOOLNO=0] THEN M81L70 (No Pre Dadoing Required)



S[DADOTOOLRPM] (Spindle Speed)
T[DADOTOOLNO] M3
M31 (verifies tool is up to programed speed before continuing)

[Daniel Vonderheide]

The M00 code is a program stop. It will stop the file from running until you press the cycle start button again. You should be fine to press the green button and continue from what I can see.

[Brad McIntosh]

I am going to go out on a limb here are make a guess...

My guess (from the comments in the code) is that this program was originally for producing SLATWALL with a T-Slot tool. As such, it would want to cut out the perimeter and square up the parts with an endmill, remove any waste that could interfere, square it back up in the corner of the G901 and then cut the T-Slots with the T-Slot cutter - which need to enter laterally from the side.

The point that you are indicating is the "remove any waste, square it back up in the corner of the G901" section. The machine is waiting for you to:

• Turn off the vacuum.
• Remove any waste from around the perimeter.
• Relocate the part back snugly into the G901 corner.
• Turn the vacuum back on.
• Press [START].

I do not see any pending input and there may be none. I would like to see the entire program as it seems we are missing the first section. If you can attach the whole thing or email me a copy, I can take a better look.

[Brad McIntosh]

I see Daniel beat me.... (Me 2 slow. lol)

[Will Williamson]

Daniel Vonderheide is the number one reason for my Great satisfaction with my Thermwood Router and Thermwood Corporation period.
And I'm really glad to see Your contributions on here Brad
Thanks Will Williamson

[Brent Riley]

The M00 code is a program stop. It will stop the file from running until you press the cycle start button again. You should be fine to press the green button and continue from what I can see.

Yes, I have resumed the program, expecting it to switch tools and start grooving. It however just loops through to the same position in the GCode again.

I will try tonight to switch the vacumn off and on again as is suggested in a later post. I wouldn't think the supercontroller detects that but its worth a shot.

I am guessing the G901 is the furtherest corner from Home?

When the program starts, it does the cutout fine. Right around the correct dimensions. Its just the transition to the Vee Groove. I have also looked at skipping the cut out process but it still comes up with the loop when I expect it to Groove.

I might also try some different measurements, it could have an error in the logic for spacing out the grooves.

Is it permissible to post full code on here? Most the code I have on the machine has a copyright saying This program is not to be reproduced without the prior written consent of Copyright Owner. Its Thermwood Corporation code.

[Brad McIntosh]

Brent,

Where is this program from? I am not sure if I would worry about a ASCII text, NC program being "copyrighted". Now the application that generated or runs that program is another matter.

If you can, just ZIP up the NC program and upload it here. They we can get the big picture.

[Brent Riley]

https://docs.google.com/document/d/1ChG ... e-sm0/edit

Im running on a C40 Thermwood CNC. Windows 2000 system. Im a bit new to the thermwood but have managed to get Flycutting and processing jobs from THM down to half a millimeter. Previously the last operator was using a sac sheet with every board. I am able to have 10-20 sheets cut before replacing the sac sheet.

Im more used to smaller industrial metal CNC cutters and lasers but finding the switch to a big machine an exciting challenge.

[Daniel Vonderheide]

After you press the cycle start to perform the slatwall cuts, there is only one line of code that has the ability to cause it to skip past everything to the end.

IF [DADOTOOLNO=0] THEN M81L70 (No Pre Dadoing Required)

THis line has it jump down to the end where it loops back to the beginning of the outline cut if the count is not zero.

M80L70




M80L90

[REP_COUNT=REP_COUNT-1]


IF [REP_COUNT=0] THEN M81L99
G990
G90G00Z0
M05
G00X0Y0
M81L30

The label 30 should be jumping you to this location.

M80L30



[CLS]
[PRINT " Ensure that the wasteboard Handling Sheet is in position."]
[PRINT " "]
[PRINT "Position the sheet material into the G901 Part locator."]
[PRINT " "]
[WINDOW ON]
M00

If it is looping you back to a different location< i would look to see if the code on the machine matches what you sent or if there was a line altered to loop it back to the M80L43 which is the beginning of the slattwall operation.