Hey all,
I have been using the CF Pro for a few months now with a Hypertherm 45xp (Machine torch with standard 45xp consumables). Things had been going okay with only a few hiccups here and there. I chalk those up to me just learning more about CNC in general. For the record, I used the standard Crossfire for a year with no issues and everything came out great.
Fast forward to today. I have spent the last few days and wasted a full sheet of 16ga material trying to cut a custom sign. I’m using:
- same computer (Win10 Pro, Intel i7 3.4GHz, 16GB RAM, NVIDIA GeForce GT 1030 Graphics card)
- same computer location
- same high-quality USB cable between computer and Crossfire
- The chokes are installed around 3 coils per Langmuirs instructions
- Latest FireControl and THC firmware.
- Sheetcam
Material is 16 gauge steel, using the Hypertherm default cut chart settings for material/consumables.
I get this error:
error|644x444
I have a shared Dropbox folder:
that contains the following:
- the .svg
- a word document containing the full error
- the .tap file
- the saved sheetcam .job file
Please help!
What versions of the Firecontrol and THC driver are you running?
Anything in the log? cut n paste this into a File explorer:
%USERPROFILE%.FireControl
then open firecontrol.log
Can you run through the program without error with THC off and plasma OFF? (have a sheet on table).
That error seems to crop up from a torch misfire, let’s assume that it is not interference.
Check your consumables, make sure retaining cap is not over tightened (this is known cause of torch misfire, distorts the swirl ring) and no corrosion (see this thread).
1 Like
Hi Greg,
I placed the firecontrol.log in the dropbox folder.
Firecontrol - v20.3
LS THC - v1.09
Machine - Crossfire v1.1ls
Yes, the program runs to completion without the cutter and THC on.
Dale
Looks like you are up to date.
Since you haven’t had interference problems before now, I’d concentrate on the plasma. I assume you have good dry air?
Have you inspected the consumables? Check the tightness of the retaining cap?
I’d start with some straight line tests with THC off. If you can get through those, repeat with THC on.
1 Like
Right before I started cutting the design I had used the straight cut option in Firecontrol to trim some of the excess off the sheet. That was with the THC on and the cuts looked good.
After I get another sheet tomorrow, I will start with new consumables and see what happens.
I took a look at your gcode:
H0; THC off (On all corners)
G92 Z0.
G38.2 Z-5.0 F100.0
G92 Z0.0
G0 Z0.2
G38.2 Z-5.0 F10.0
G92 Z0.0
G0 Z0.02 (IHS Backlash)
G92 Z0.0
G0 Z0.15 (Pierce Height)
M3
G1 Z0.06 F60.0 (Cut Height)
The above is line 7 to 21 in the file. This would be the start of your first cut.
Unless I’m missing something, I don’t see the pierce delay.
After the M3 line there should be a line that looks like:
M3
G4 P0.6
G1 Z0.062 F50.0 (Cut Height)
With the G4 for the pierce delay.
This looks like you have a rule defined to turn off the THC. Is this something you used before?
I’ll take a look at your job file… but I think this is probably your problem.
1 Like
Greg,
You are correct. I added rules in for slowing down at some corners and turning the THC off/on trying to make the tighter corners a little cleaner. I’ve used the rules before, but not to this extent. If the pierce is not there, I can’t explain that one.
Dale
I took a look in the debugger for the post in Sheetcam and the pierceDelay is 0. I created a clean job file, imported the svg and got the configured delay. So this seems to be a bug in the job file/sheetcam. I’ve started a thread on the Sheetcam forum here
Can you confirm what version of Sheetcam you used to make the job file?
Greg,
I’m using Sheetcam 6.0.30.
Dale
Greg, you are what the spirit of this forum should be all about. Posting a question on another products forum to help a Crossfire customer! Unselfish help for those in need. Bravo!
3 Likes
You can use sheetcam rules to slow down for corners / holes smaller than x" but don’t have sheetcam tell firecontrol when to shut off THC. Firecontrol will do that for you when it sees the speed reduced.
1 Like
I went through and removed all the THC ON/OFF from my rules and reprocessed a fresh import of the svg without saving. Everything was going fine, then at line 8149, I get the error again. That was my last piece of metal to try with until I can get back to the supplier. I had put in new consumables before cutting also. The application is then locked and I ultimately have to use the “quit task” option to closed it and restart.
Did you verify if the generated gcode had pierce delays?
Please post the latest generated gcode (use the button with the arrow on it above where you type your reply to attach it). Then we can see if it has pierce delays.
Greg,
It looks like there are Pierce Delays in it.
DesignV2.0.tap (237.1 KB)
Dale
I don’t see any pierce delays, I see G4 values for your after cut delay (0.5 sec) but nothing for the pierce. The pierce delay would see an M3 (torch on) followed by the G4 (delay). 16 gauge is probably forgiving and piercing during the move from pierce height to cut height, which is why you are able to run most of the program. But this isn’t how you want to run.
Line 8149 is during the IHS routine. So hard to know if it really happened there or what is going on.
I can’t say for 100% the no pierce delay is the problem, but you should have that working before moving on.
I would wait until I heard back from Sheetcam before burning any more steel. While waiting, are you running with Smart Voltage or have you specified a voltage? Langmuir recommends not using Smart Voltage on material less than 14 gauge, see Lost arc again! - SOLVED
You might want to do the line tests and dial in a voltage. But I would NOT cut anything else until you get a proper post with the pierce delays.
1 Like
That was my misunderstanding, I thought the G4 was the pierce delay. I’m still learning about the G-code format. It sounds like I need to wait until I hear something back from the Sheetcam forum you posted on before proceeding…
I have had plenty of projects where the output was great, but there are a couple now (more complex designs) where I have issues.
I can’t thank you enough for your assistance!
I am using sheetcam also. Here is what a chunk of my gcode looks like. If you go to the file location where you save the gcode and open it in text format you will see notes that aren’t displayed in the firecontrol window. This helps you understand the code a little better.
(SheetCam - FireControl Post v1.5)
G90 G94
G17
G20 (Units: Inches)
H0
G0 X0.686 Y0.4162
G92 Z0.
G38.2 Z-5.0 F100.0
G92 Z0.0
G0 Z0.2
G38.2 Z-5.0 F10.0
G92 Z0.0
G0 Z0.02 (IHS Backlash)
G92 Z0.0
G0 Z0.15 (Pierce Height)
M3
G4 P0.6
G1 Z0.06 F60.0 (Cut Height)
H1
G3 X0.75 Y0.3523 I0.064 J0.0 F90.0
G3 X1.1478 Y0.75 I0.0 J0.3978
G3 X0.75 Y1.1478 I-0.3977 J0.0
G3 X0.3523 Y0.75 I0.0 J-0.3977
G3 X0.75 Y0.3523 I0.3977 J0.0
G3 X0.78 Y0.3534 I0.0 J0.3978
G3 X0.839 Y0.422 I-0.0048 J0.0638
H0
M5
G4 P0.5
G0 Z1.0
G0 X6.1306 Y0.4525
The P0.6 between the Pierce Height and Cut Height is the pierce delay that Greg is talking about. If you notice lower in the code there is also a P0.5 before the z1.0. This is a pause that I have in sheetcam. It will pause for .5 sec. after every cut.
Thanks for the explanation. I think I better understand. So, I don’t know why Sheetcam is not writing this out then. On the latest version, I imported the svg and chose a new tool for the operation to try on some thinner material, but it appears the pierce delay is not getting written.
Can you post a picture of the tool settings in sheetcam that you are using for the 16ga?
It is something to do with your job/tool file combination. I’ve attached a ‘clean’ job file to start from, that I did, where I get the pierce delays. But you will need to redefine each of your rules and your tools. I would do one at a time, run the post, verify pierce delay, then define the next. Save the job file to a new file name at each step (job1rules.job, job2rules.job etc). This way we might be able to figure out what is tripping Sheetcam up.
Under View turn on Code Editor. This will pop up a window each time you run the post with the GCode in it. You are looking for M3 followed by G4, that is the pierce delay. See below.
fordaleworks.zip (339.1 KB)
