Modifying post

ajclay · Post by **ajclay** » Sun Mar 30, 2014 6:39 pm

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.

Thank you for all the help.

AJ Clayton

Post by **Les Newell** » Mon Mar 31, 2014 12:14 pm

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.

ajclay · Post by **ajclay** » Sat Apr 05, 2014 6:21 pm

Thanks for the info..

Another Question.

Les,

What's putting the "S20" code in my post when the "small hole" rule
specifies DTHC OFF S10?

The torch doesn't need the DTHC ON for cutting these holes.

Is this normal operation for SC to put in the S20?

Thanks for the help and information. I'm trying to get a handle on the
advanced operation.

Attaches are my files...

AJ

-----Original Message-----
From: Les Newell [mailto:forumadmin@forum.sheetcam.com]
Sent: Monday, March 31, 2014 7:14 AM
To: problems@forum.sheetcam.com
Subject: Re: Modifying post

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.

Post by **Les Newell** » Sun Apr 06, 2014 8:37 am

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:

Code: Select all

--THC on and off codes. Use nil if you don't want THC control e.g&#58;
-- 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

Code: Select all

--THC on and off codes. Use nil if you don't want THC control e.g&#58;
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"

ajclay · Post by **ajclay** » Mon Apr 07, 2014 7:07 pm

Les,

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....

Take a when you have a spare minute.

The simple things are the hardest it seems...

Thanks, AJ

-----Original Message-----
From: Les Newell [mailto:forumadmin@forum.sheetcam.com]
Sent: Sunday, April 06, 2014 3:38 AM
To: problems@forum.sheetcam.com
Subject: Re: Modifying post

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"

Post by **Les Newell** » Tue Apr 08, 2014 12:07 pm

The current dev version has some issues when editign posts. These will be fixed in the next release.

ajclay · Post by **ajclay** » Sun Apr 20, 2014 3:40 am

Les,

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 attached the post, job, and tap file.

As Always, Thank you for the time.

Aj

ajclay · Post by **ajclay** » Thu Apr 24, 2014 11:11 am

Les,

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.

One minute video here:
https://www.youtube.com/watch?v=tvxFnOWiNl0

In the DRO:
Notice lines: N0300, N0340, N0380 all on inside contour
Outside contour, Notice lines: N0620, N0660, N0700

Any ideas? comments?

attached is the tap file.

Thank You !

Aj

Post by **Les Newell** » Thu Apr 24, 2014 3:03 pm

Could you try this with the latest Stable V6.0.1. It may help.

SeanP · Post by **SeanP** » Thu Apr 24, 2014 3:15 pm

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.

Video of mine using the same job file is much the same as well.
https://www.youtube.com/watch?v=ez0mRN2dru8

Post by **Les Newell** » Thu Apr 24, 2014 3:34 pm

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.

SeanP · Post by **SeanP** » Thu Apr 24, 2014 3:36 pm

Thanks Les, will give that a try and report back.

SeanP · Post by **SeanP** » Thu Apr 24, 2014 3:56 pm

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.

Thanks
Sean

Post by **Les Newell** » Thu Apr 24, 2014 4:58 pm

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.

SeanP · Post by **SeanP** » Thu Apr 24, 2014 5:50 pm

Looking good now Les!
I un-installed/reinstalled still the same on 1st try.

Then I deleted the settings folder (help menu/settings folder) and reinstalled
now code is produced like you said it should be.

Not done any testing yet, we have a better chance now though.

Thanks a million, nice easy fix.

Sean

sheetcam.com

Modifying post

Modifying post

Modifying post

Modifying post

Rules not working

Good news