My first NC question... be gentle

[Simko]

OK... I have my CandCNC setup on the bench and I am attempting to get it to run properly before putting it on the actual table.

Everything seems to be working great except that I can't get the motors on the bench to run at 'full-cut speed' after the first cut. For example, when I run the g-code, it does a rapid to the first cut, then it makes the first cut at whatever speed the tool is set to run at, then all subsequent cuts are made at 20 IPM....

1) All of the motors are hooked up and work properly when jogging
2 I added a limit switch for the z touch off that I trip manually when it goes to do each touch off while running in AUTO
3) I loaded this DXF into SheetCAM (http://plasmaspider.com/viewtopic.php?f ... 15#p112528)
4) I loaded the LCNC_Hypertherm45-105+codes.tools toolset
5) I picked T1-45A-26ga steel tool
6) I created a new jet cutting operation

screenshot.png

7) Run the CandCNCPlasmaLLCNC-rev14 post processor, save TAP file
8) Load TAP file in CommandCNC

screenshot2.png

9) Zero everything, press RUN, motors rapid to first cut, starts touch off, manually trip z-switch
10) The first cut is made at 350 IPM
11) Rapids to next cut, starts touch off, manually trip z-switch... the cut is made at 20IPM along with all the rest of the cuts

Attached is the TAP file...

Punisher skull with ar15s.tap.zip

I'm sure it's some setting that I don't know to set... any help would be much appreciated. Hopefully I can work through this learning curve quickly.

Thanks!

[acourtjester]

I am assuming the G-code should be the same as Mach so if you look at the speed commands they will be after the position instructions (G0 or G1) along with with what axis it is moving. As you said the first is 350 IPM so that speed command is F350 look down the G-code the touch off speed will be less and then speed back up after that for the next cut operation. I know mach only changes speed by command. your g-code may not be changing speeds after the second touch off. If there is no new F commands you will not change speeds.
example
G1X5.09Y12.4F350 this is to move the X to 5.09 and the Y to 12.4 at 350 IPM

[Simko]

That is exactly how it is acting! There must be some setting that I am missing in SheetCAM to set the speed on all the cuts to the rated tool speed.

[islander261]

Hello

Acourtjester is correct.

The F (feedrate) command is modal. This means that once it is set by a command it stays at that feedrate until it is changed by a new feed rate command. When you touch off you are setting a slower feedrate so you don't smash your torch into your work then after your touch off you (Sheetcam) didn't reset the feedrate to the correct speed. The problem is in your Sheetcam settings or post, most likely in your settings. You can manually fix the file if you want to by adding F350 to the first movement block (command) after each touchoff.

John

[acourtjester]

In SheetCam you set the feed rate for each tool and after you modify the tools you must save the changes by saving the tool sets. Wither by giving it a name you choose or "save default tool set". If you use you use your name you must load that each time you run SheetCam. If you save it as default it will load that each time normally.

feedrate.jpg

feedrate1.jpg

[tnbndr]

Also, any time you make a change or edit a tool you must re-apply that tool to the item. It does not automatically update.

[Les Newell]

This is a bug in the post processor. I don't have a copy of that post but it looks like the post is written to output this line as simple text:
G38.2 Z-0.50 F#<_hal[gscreen.toffrate-s]>
As it is just text the post processor has no way of knowing the feed rate has changed. If you post a copy of the post processor here I'll fix it for you.

Also, any time you make a change or edit a tool you must re-apply that tool to the item. It does not automatically update.

This will happen for some parameters such as feed rate. Feed rate on the tool definition is just the default value and it is quite common to change it in the operation to suit your specific task. Parameters like this will have an 'update operations' button next to them. This button will apply that parameter to all operations using that tool.

[Simko]

It is looking like it may be a problem with the POST processor. Les from SheetCAM asked that I post it here to keep everything in one place.

Here is a link to the POST

http://candcnc.com/images/downloads/Can ... -rev14.zip

[Les Newell]

It was a bug in the post. I have attached a fixed version.

[Simko]

THANK YOU Les!

I will try it out right now

[Simko]

It works great... Thanks a lot Les!

Now the only big remaining issue is to figure out why I can't cut a whole file without getting an X / Y / or Z following error in CommandCNC.

[exapprentice]

Hi Steve

mmmmmm

How did it go hope Les got it sorted, seems like your having a bit of a nightmare at the moment.
Keep calm and breath its only money, could be a lot worse.
I am sure things will get sorted, when I can remember when I first set up my machine the pain and all those questions in your head.
It should be so simple and straight forward , why me, I know I did what it says on the tin or did I
things look very dark at the beginning but there is light at the end of the tunnel, you just have to walk a bit further to see it
good luck and keep going, let us know how things progress

[Simko]

I did a little more testing this morning and the POST is working great. I can only assume that anyone else running CommandCNC with CandCNC electronics would have the same issue and should probably download the updated POST that Les modified.

I also got an email from Moses at CandCNC last night saying that he has seen similar 'following error' issues and it was identified to be a USB keyboard and/or mouse that caused the problem. I changed out the mouse and ran the Punisher file a few times and did not have ANY X/Y/Z following errors. I will do more testing, but it looks promising as I wasn't able to get more than six cuts into the file before I changed the mouse.

I may have also figured out the file close issue, but I would like to verify with someone who is running CommandCNC. Whenever I would try to close a file I would get an error saying "File ended with no percent sign" and "Can't open blank.ngc". I found where the blank.ngc file was saved (it was completely blank) and put an M2 (program end) code on line 1 and now I can close files without error. Would someone be able to verify what is actually supposed to be in the blank.ngc file. It works with an M2 (program end) or an M30 (program end, return to start) code.

Thanks for the words of encouragement Exapprentice! Things are starting to look more promising and I am able to breath a little easier now..

[motoguy]

Is CommandCNC working well for you now?

[tcaudle]

REV16 post now supplied fixed all of the feedrate issues and the 0.6.1 update fixed the :Close" The iusse in LUNUX is that there is not such thing as a "Close:, it simply opens up a blank file in place of the one to close.