Command CNC torch height jumps UP

[TJS]

CandCNC has their own forum. They also have many documents in digital form you can grab from their site, as well as the most recent posts to download. I suggest posting your concern over there. There is a learning curve but once you get all the parameters set you will be happy. The owner of Candcnc also hangs out here and posts here as well. The next tab over is the diagnostics screen, what does that denote. I had an issue with one of my switches and I used that screen to pinpoint and diagnose what was the culprit. It kept telling me the Y limit had an issue. I then got the ohm meter out and checked continuity and had a wire issue right at the switch.

[tcaudle]

If you can't cut in MANUAL mode then its not a DTHC issue. If you will go to our website and the SUPPORT Section you will find MANUALS on everything we sell. The one you need to dig into is the DTHCIV Setup and Config . Its over 130 pages . Don't get intemidated. You may also want to download the DTHC 5 Troubleshooting Guide document too . Go to the section (about page 85) that has INITIAL CUT TEST. There are specific tests you do one at a time. It will narrow down the problem. First test does a simple touch off and move to pierce height. ALL of that is from g-code and settings in SheetCAM . No DTHC involved at all . If you cant get a correct touch off and move to pierce height you will NEVER get the DTHC system it cut.

We have an RFS (Request for Service) form in the SUPPORT section that goes directly to Engineering.
Judging from the errors you are getting, lots of stuff is not setup correctly . The G38.2 error that says it did not find the sensor is because either the sensor is not working at all or the readout is so far from zero top of material that it went past the preset -.75" limit .

SO run the Initial Cut Test steps and STOP when one fails and contact tech support or use the RFS. The RFS is handy because it gets answered after hours and weekends versus phone support Thai is business hours.

you dont have to name names here but we would like to know the name of your table builder. We typically support the OEM first but if they drop the ball or cant answer the issue then we are always here to support our products. A random builder is not an OEM .

On of the things I see that MAY or may not be involved is your torch volts show 0. That is normal if you do not have the torch fired but then the HOLD and Delay should not be on. If it fired then went out the control still see the torch fire signal and is waiting for the ARC OK to tell it to release and proceed. HOLD means its not getting an ARC OK there are parameters in SheetCAM in the tools that define pierce height and cut height at the beginning even without the DTHC active. You can also send the G-code you are trying to use to us and it will be obvious if some settings are wrong

Our online support form will get you more precise help and faster feedback.

[TJS]

According to your screen shot of Command CNC You Hyt License is not found. Not sure if this matters at this point in time.

[tcaudle]

That has nothing to do with the issues he is having. It simply tells him that IF he has the Optional HYt-Connect RS485 connection tot his Hypertherm it will not set Current or Air pressure from Code. It cannot cause any of the errors. I doubt he has that option installed and even if he does unless its hooked up and shows up in the Hub utility as a DEVICE it will just ignore the settings and cut in normal Manual mode at the Hypertherm.

[Deezl Smoke]

I think we need to create a couple path rules. Or at least see what "none" has under it.

Lots of great pictures. Probed tripped during homing motion is an adjustment I think.

On the desktop, is there a icon like "utility hub" or similar? If so, double click on that and see if any components are recognized.

[tcaudle]

Path rules are dnagerous in SHeetCAM . A LOT of the automation is internal path rules and if you stick in outside path rules thye tend to do strange things. The only Path rule we suggest os the EOC (End of CUt)
User has not made any contact via website or RFS so maybe they are using the manual and the Initial cut Test to get things set correctly
There will be a desktop ICON for Hub Utility (icon of a hub) . It should be run with CommandCNC NOT running as both try to talk to the hub at the same time on the same channel.

[Deezl Smoke]

Path rules are dnagerous in SHeetCAM . A LOT of the automation is internal path rules and if you stick in outside path rules thye tend to do strange things. The only Path rule we suggest os the EOC (End of CUt)
User has not made any contact via website or RFS so maybe they are using the manual and the Initial cut Test to get things set correctly
There will be a desktop ICON for Hub Utility (icon of a hub) . It should be run with CommandCNC NOT running as both try to talk to the hub at the same time on the same channel.

So just for the where I'm coming from info, I use Qcad to draw, Sheetcam to generate code and Command Linux base like the OP here.
For me and how I use this equipment, I need a few path rules to Keep the DTHC from diving the torch. Like on circles smaller than """ turn DTHC off etc. I also use a path rule for slowing on corners and turning the thc off for the corner then back on again. My limited knowledge of this equipment doesn't allow me to know how else to do that.

This morning I fired up the machine for a quick cut job. Was working fine last night for a few test pieces for the press brake. This morning however, same parts and settings, just a larger array, no go. I did get it running, but the issue was similar to this thread which is why I'm mentioning it here.
This picture shows the controller already attempting to cut. Each hole, the torch would dive into the plate at end of cut. Even though there is a path rule telling it not to do that. So I tried the outside offset and the torch would just dive into the plate even though the DTHC was on and working. The preset voltage for 45amp steel should be 136 or 7 volts.

So I stopped and opened the hub utility.

After pushing the reset button in the hub, this is how it should look.

Anyway, took a bot of doing with a separate path rule to deal with radius corners, but got it all working. I just don't know why the hub, which a new component, did not recognize the other components.

[adbuch]

Thanks for that information Deezl Smoke! I know that some folks cut the holes as a separate operation using a slower speed, then cut the remainder at regular speed. This would eliminate the need for a path rule for small holes.

David

[acourtjester]

With SheetCam moving holes to a different path they can be cut as a separate operation as part of a complete G-code. They would be cut as a inside cut path and the rest as outside path cut with different speeds in the tool description. I have used that form the center punching action to mark drill holes and they are cut first then other cut routines cut after.

[Deezl Smoke]

I use the "center punch" feature quite often. Love it.
My choice is to punch or cut holes first then cut the outside offset part for each part before moving on to the next part. Whereas I see you punch all parts first, then cut.

[acourtjester]

Just the way I do it not sure if any benefit to that way, It seems SheetCam will separate the routine with their inside cut first method. This makes planning simple, I just move from part to part and when I do the post processor it does the center punch first then the other cuts.

[Deezl Smoke]

Thanks for that information Deezl Smoke! I know that some folks cut the holes as a separate operation using a slower speed, then cut the remainder at regular speed. This would eliminate the need for a path rule for small holes.

David

Hoping we are not going too far off topic. We are talking about settings etc., so I think this may still be applicable to the topic,....I hope anyway.

This is how my parts look in Qcad.

So here is my single part as I import it into Sheetcam.

Then I array the parts with spacing for lead ins and lead outs etc.

In other sheetcam settings, it is set up to cut all inside first, so for whatever reason, I simply follow that concept when I apply operations.

Then outside. Note in some situations, I end up having to reduce the cut speed an inch/minute and over cut .1". I have a feeling my shop power, though a new service, is not as clean as it should be, which is why my often inconsistent quality of cut. But this is also why I rely on the thc so much.

And finally my pah rules as of current. However I did learn that the arcs and corners rules conflicted for this job as the part corners were radius. But you can see in the sheetcam pic that the outside cut has a path rule applied at the part corners.

[acourtjester]

One thing I would mention is different software/controllers use different codes, so working with cut rules that needs to be followed. These codes should be found in the manuals for the software/controller. Example I used G31 for probe command, but when I switched to LinuxCNC I now use a G38 for the probing action.

[tcaudle]

For me and how I use this equipment, I need a few path rules to Keep the DTHC from diving the torch. Like on circles smaller than """ turn DTHC off etc. I also use a path rule for slowing on corners and turning the thc off for the corner then back on again. My limited knowledge of this equipment doesn't allow me to know how else to do that.

Let me see if I can explain why Cut rules do not work well with our POSTS and CommandCNC:

If you use our POST fro plasma you will see several settings in Operations that are custom: They basically are internal Path rules that use logic to decide when to apply them. One you would see is an input box that is labelled "Min Cut Length for DTHC| and a default setting of "1" menaing 1 unit (inch in most cases) That looks at the UPCOMING shape (be it round square or any other shape and in ShetCAM every cut has a internal variable named EnityLenght that tells the POST Processor how long it is. So if you set that to the CIRCUMFERENCE + lead-in of the entity it will not even turn ON the DTHC at the beginning . The DTHC has auto ON and off on each cut . If you start sticking cut rules into the mix they will conflict. For some reason tell it to turn off twice will cause it to do the opposite . So if you set that Operations parameter to a number that catches all of the smaller cuts it AUTOMATICLLY leaves the DTHC off . You also have th eoption to put all of the holes (or even smaller ones) on a separate layer and check the box that says "Disable DTHC this OP" and nothing in that opeartion will use the DTHC. Either way lets you control the cuts with no other rules but EOC.

You will note that the one rule we included in our toolsets is the EOC pule. It designed to tunr off the TDHC on a cut as it approaches the end where it means up with the beginning. That rule is based on the total length including lad outs. I prefer not to use lead-outs in most cuts. The piece has already fallen out BEFORE it reaches the junction point of lead in and lead out so voltage spikes and feedrate has not dropped (especially whit a long lead-out) so the DTHC reacts to the voltage spike and dives. You need to make the EOC distance enough that it turns the DTHC off BEFORE it gets too close to the lead in and the piece starts to drop out. If you are getting a dive at the end of a cut its beacuse you eiter do not use EOC path rule or you have the lead out too long 9or the EOC distance too short)

OperationsOptions.png (30.12 KiB) Viewed 938 times

OperationsOptions.png (30.12 KiB) Viewed 938 times

So use the built in "rules" and forgo other rules. Now if you have some other type of THC The POSTS wil be different and they most likely do not have internal cut rules you can select from the Operations

There are two types of commands in Linuxcnc : Static (done as a line of cut and not during other motion) and dynamic that executes DURING motion and does not cause a pause.

[tcaudle]

If you have and use VAD (you can change the trigger % in the DTHC settings) you do not need a rule for corner diving. If you have the acceleration set too hot (like you had to do in MACH3) it will not start to slow down soon enough. Go inot your XY Motor settings and lower both to 20 IPS/sec and things will get less jerky and VAD will do a better job. You can turn VAD on and off on the POST but in most cases its there to STOP corner diving and it very fast. What will hurt you is setting the VAD at a lower number or if you go above 90% and keeps the DTHC off most of the time. You can tell if it woekign as it cuts beacuse the DTHC ON LED will reflect it being turned on and off. The one on the controler shows the DTHC status in the box

[tcaudle]

And if you DO use VAD and a cut rule too it will often do the opposite of what you want

[Deezl Smoke]

You lost me on VAD and POST fro. But you got me wanting to look deeper to see if I have some of the conflicts you are explaining. My power supply is a Hypertherm pm105 and my table is an Arclight dynamics. The post processor in sheetcam is also arclight's.

[tcaudle]

You should be able to tell if the PC is LINUX and if the Control screen is a CommandCNC.
I wrote their POSTS for SheetCAM and if it old it may not have the added options .

[Deezl Smoke]

It is Linux, and the program says "Command CNC"

[tcaudle]

see the check box in the THCPanel (bottom Right) that as Velocity AntiDive (VAD) its checked ON
That gets automaticity set if its set in SheetCAM

The cut rules are in the toolset . There shold be the EOC cut rule that you can select as a PATH rule and make it happen on every cut

You might want to take advantage of the mananas we have that cover CommandCNC and some of the ShetCAM. We have a SUPPORT/MANUALS section and you have 300 pages of casual reading with the Bladernner and the DTHCIV manuals for CommandCNC.

You can alos get later POST processors for the system on our SUPPORT/?DOWNLOADS sectionj . Dont update any firmware until you check with us. Your versions may not need them as far as the Hub utility and DTHC firmware

You can stop a lot of the issues you are having by changing some settings and using the built in Cut Rules. Adding outside cut rules is NOT going to work well. Putting a corner cut rule may defeat internal cut rules or vice versa.

One thing : DO NOT use the FRO (feedarte override slider ) when using VAD because it will mess things up and cause it to turn off when it should not. Its fixed in later COmmandCNC releases but that is probably a 32 bit version and is not a simply upgrade

[Deezl Smoke]

see the check box in the THCPanel (bottom Right) that as Velocity AntiDive (VAD) its checked ON
That gets automaticity set if its set in SheetCAM

The cut rules are in the toolset . There shold be the EOC cut rule that you can select as a PATH rule and make it happen on every cut

You might want to take advantage of the mananas we have that cover CommandCNC and some of the ShetCAM. We have a SUPPORT/MANUALS section and you have 300 pages of casual reading with the Bladernner and the DTHCIV manuals for CommandCNC.

You can alos get later POST processors for the system on our SUPPORT/?DOWNLOADS sectionj . Dont update any firmware until you check with us. Your versions may not need them as far as the Hub utility and DTHC firmware

You can stop a lot of the issues you are having by changing some settings and using the built in Cut Rules. Adding outside cut rules is NOT going to work well. Putting a corner cut rule may defeat internal cut rules or vice versa.

One thing : DO NOT use the FRO (feedarte override slider ) when using VAD because it will mess things up and cause it to turn off when it should not. Its fixed in later COmmandCNC releases but that is probably a 32 bit version and is not a simply upgrade

Thank you for that statement. That is an issue I have. intermittently when opening the program, that slider will be at 95%. I then hit reset and it goes to the needed 100%. That is, at this point it is the needed percentage. I will as time allows me, go check out more on your site.

So I will look into the VAD setting. For some reason, I don't recall seeing it in Sheetcam, but in one of the settings icons in Commandcnc. I'll look.

[tcaudle]

VAD is not in SheetCAM except as an option (on.off) in Operations IF you use correct POST

YOu can only set the VAD % in CommandCNC THC SETTINGS tab . Default is 85%. good for most cutting. Do not go over 90% or less than 80 or it can not work like its supposed to. VAD monitors the REAL feedrate and will stop DTHC aciton asl long as the actual feedrates is less than the percentage you set. so lets say your commanded feedrate is 100 IPM . If the REAL feedrate hits 85 IPM or less the DTHC turns off and the Z does not move. Once it oes back to 100% it turns back on. By lowering the motor tuning acceleration number the tool path trucking in CommandCNC will force the machine to slow down sooner on turns and arcs .

The only time that you need to turn off the DTHC in full speed cutting may be on a small object or at the end of a cut where the leading and lead out cross. Usually the piece starts to dropout before the lead out is hit and the voltage spikes during the lead out , The EOC cut rule turns the DTHC off BEFORE you get to the place kerbs cross or a bigger piece start to dropout and you get a voltage spike.

if you are getting torch dive at the end of a cut you have a setting that needs to be changed or you need to confirm the DTHC is being shut off. You can see it in the code in the motion calls for XY. There is be a dreaj in the code and the M67 E0 Q10 is called to disable the DTHC in the posiiont of that cut. The software (SheetCAM) knos where in the line to insert the code . It keeps a running value of the distance to the end of a cut . Keep in mind if you have a long lead out you want to turn off the DTHC BEFORE it get too close to where the kerf gets close to the lead in kerf , NOT to the end of the lead out. In short it best to turn it off sooner than later (unless you are cutting HVAC or corrugated .

I seldom use a lead out. They only time to use them is if you are getting a divot at the end for when the torch stops but the flame stays on for a short time after OFF is sent.

[Nuke Utter]

Thanks for all the help! the dude that sold me the table has helped me out a bunch. Info overload! this is a lot to take in. Unfortunately I learn better from hands on, and the manuals are hard for me to digest.
I do have the machine cutting better. I am still having issues with dimensions off setting from fusion to sheet cam and cutting out on duplicate parts.
I found my main problem was the crash sensors needed fine tuning, but I messed with my settings getting me in a pickle. Mostly just newbie errors and settings needing to be re-adjusted. I'll get it in time and a lot of plate!
I really appreciate all the responses and if anyone lives in southern, Alberta and wants to give lessons!

[adbuch]

Nuke - glad to hear you've got things sorted out and are back to successful cutting. Be sure to show us some pictures of some of your projects.
David

[tcaudle]

I cant address using fusion 360 for plasma and 2D drafting. I do know if the table is correctly calibrated and motors are tuned correctly it will cut very accurately . I would suggest that you do some design in either ORCAD or Inkscape and nest the shapes in SheetCAM. Just as a test . You can run a simulation of the cut in SheetCAm and at least see if its going to cut like you think.
Now I need to go figure out what a crash sensor is......