Les, I’m using a post that Tom at CandCNC has modified. It’s used for a plasma unit that has the computer output in rear. I have an older power unit that is set manually.
The post works well with the exception that I get a M00 in the code because it’s not receiving the needed info. I have to hit run a second time to get the machine to run.
Would you be so kind to make a quick edit in that post to keep that from happening? Or tell me what needs to be changed.
Edit the post and look at the end of the file. Near teh end of teh file you should find these two lines:
post.Text (" M00\n")
post.Text (“(Check the DTHC Settings Hit RUN to continue)\n”)
Delete them or put two minus signs (–) before them. Two minus signs tell Lua to ignore the rest of the line.
Edit the post and look at the end of the file. Near teh end of teh file you
should find these two lines:
post.Text (" M00\n")
post.Text (“(Check the DTHC Settings Hit RUN to continue)\n”)
Delete them or put two minus signs (–) before them. Two minus signs tell
Lua to ignore the rest of the line.
That is being generated by the post. This post was written before path rules and tries to do what path rules does. Edit the post. Near the beginning you should see this:
--THC on and off codes. Use nil if you don't want THC control e.g:
-- thcOnCode = nil
-- thcOffCode = nil
--these codes are for the DCC extensions and turn the DTHC on/off if you have DTHC REV1/4 or higher firmware
thcOnCode = " S20"
thcOffCode = " S10"
Change it to
--THC on and off codes. Use nil if you don't want THC control e.g:
thcOnCode = nil
thcOffCode = nil
--these codes are for the DCC extensions and turn the DTHC on/off if you have DTHC REV1/4 or higher firmware
--thcOnCode = " S20"
--thcOffCode = " S10"
I had it working and now I’m getting post errors… Sometimes after I run the
post processor in SheetCam I get an error in the gcode, and other times when
I’m trying to edit the post and try and save… experimenting…
That is being generated by the post. This post was written before path rules
and tries to do what path rules does. Edit the post. Near the beginning you
should see this:
–THC on and off codes. Use nil if you don’t want THC control e.g:
– thcOnCode = nil
– thcOffCode = nil
–these codes are for the DCC extensions and turn the DTHC on/off if you
have DTHC REV1/4 or higher firmware thcOnCode = " S20"
thcOffCode = " S10"
Change it to
–THC on and off codes. Use nil if you don’t want THC control e.g:
thcOnCode = nil thcOffCode = nil
–these codes are for the DCC extensions and turn the DTHC on/off if you
have DTHC REV1/4 or higher firmware --thcOnCode = " S20"
–thcOffCode = " S10"
I’m not understanding some little something. I’m trying to use Rules for turning DTHC off during small arcs and then back on after.
The tap file looks correct to me. And in SheetCAM simulation, it seems to show up correct too, but there isn’t a little window telling me when the DTHC is on or off. I’m just going by the colors on the contour.
I’m running the new stable version and not the dev version.
During cutting of the simple contour, DTHC gets turned off before the arc, but it doesn’t come back on afterwards. I have to manually turn the DTHC back on after every corner.
Any suggestions on what to investigate. I’m running the latest version of
Mach3 - R3.043.067
I’ve made some progress on trying to run a program with rules in the g-code.
Of course it works in simulation mode in SC just fine.
And it works in Mach when I “single step” each line. The S codes are read and they toggle the DTHC on and off.
But here’s the twist. When tap file is running at speed, on some g-code lines the S code don’t show up in the DCC Action Code window till the end of the g-code movement. So it doesn’t toggle the DTHC on and off till it’s to late.
During the first movement of the g-code on the contour it works correctly, but on the remaining three arcs of the square it doesn’t.
I am finding the same as AJ Les, we have both been trying to work together to try and suss out these rules, I am running the same software as AJ, both of us are using the new 6.01 tng version.
Try manually editing the g-code and putting the moves on a separate line. For instance change:
N0220 S10 (DTHC-OFF) G03 X1.8694 I-0.2263 J-0.2263 F31.5
to
N0220 S10 (DTHC-OFF)
G03 X1.8694 I-0.2263 J-0.2263 F31.5
repeat for the rest of the file.
I just tried that Les, first rightly or wrongly only did the off commands and that wasn’t right, so did the on & off and it ran perfectly.
AJ will be chuffed as I am it’s the first sign of progress in a while.
Hope you can work something out with that.
I can’t understand why SheetCam isn’t doing that automatically. I just tried it here with 6.0.1 and it put the thc on/off commands on their own lines as expected. Just in case your install is messed up, restart your computer then download and install 6.0.1.
I have attached a copy of the post with the dthc stuff removed. I have also attached the generated code.
I have SC installed on two separate computers, Home and work. Both I let do auto updates and use the same tool set. Both are the newest version of sheetcam as you mentioned. I wouldn’t think the program is corrupt, but that sure would be an easy fix…
I get the same code from both computers. Same post… S codes are always mixed in with the x-y movements.
I am extremely excited about the progress that you and Sean have made. He and I both have countless hours invested in trying to learn all we can about SC and Plasma cutting.
I’ll use your post and try the tap file to see how things work out…
It’s so nice to know that the problem is at least verified…
I have been running the same post processor also. MP-3000 DTHC 11 scriber (DTHC 1V setup) The last version looks like it fixed the S-10 /S20 commands. It was not putting them in quite right before. I still can’t seem to get the slower hole cutting speed to show up in Post with rules. Had it set for 75 % reduction on holes less then 1.5 inch. I was only looking at the Code, and not cutting anything with it yet. Mostly there, and easy to edit that one on simple drawings…
OK figured that one out, So everything looks good now… Been away from this a bit, and it’s coming back slowly in how to do things. SheetCam is always good about poking around ,and finding what you need.(Or Les will find a fix for you) Can’t wait for my Camera for the Scannything!
After a good few hours head scratching and comparing settings with the house pc (which was working fine) I have found what is causing the problem.
In path rules the tick box ‘show path rules in g-code’ if I tick that, the s code doesn’t go on a separate line, unticking it outputs the code just fine.
I would have had that ticked previous to the last reinstall as well.