CandCNC thc with industrial plasma (hypertherm ht2000)

[DanOSB]

I am wondering will either thc below

http://www.candcnc.com/LCTHC.html
http://www.candcnc.com/UBOB.htm

will work with high frequency plasma cutter (ht2000)
https://www.hypertherm.com/en/Produc...sma/ht2000.jsp

also second question.. i was comparing the difference between lcthc and dthc

one of difference for Torch Volts Resolution for dthc is 0.25 volt while the lcthc is 1 volt

is that adjustable importain for larger industrial machine?

Thanks
Dan

[Torchhead]

I am wondering will either thc below

http://www.candcnc.com/LCTHC.html
http://www.candcnc.com/UBOB.htm

will work with high frequency plasma cutter (ht2000)
https://www.hypertherm.com/en/Produc...sma/ht2000.jsp

also second question.. i was comparing the difference between lcthc and dthc

one of difference for Torch Volts Resolution for dthc is 0.25 volt while the lcthc is 1 volt

is that adjustable importain for larger industrial machine?

Thanks
Dan

1. Either system will work with HF start units. Both have total analog isolation of the torch volts from any PC side logic. Both are Digital
2. LCTHC is designed to add to existing tables. It has all the controls on the front panel
3. MP3000-DTHC is designed to build a system around (motor drive signals. expanded I/O, etc.) It does not require any other BOB or cards. It uses the UBOB as it's Brekaout Board technology
4. The DTHC has features like Cut Profile list, on screen setup and readouts and various DTHC parameters that be set.

The DTHC system is capable of holding very tight voltage/height IF the Z dynamics are good enough.

The DTHC will continue to have features added (i.e. Digital Current Probe, Auto-Learn Cutting, and others. The LCTHC is limited to what it currently has.


TOM caudle
www.CandCNC.com

[koh]

Tom,
What G-codes on and off THC (MP3000-DTHC) from the control program ?

I need to disable the THC before cutting small holes. and then again to enable THC. How do G-code to do this?

[Torchhead]

THC logic is turned on/off in MACH (not at the DTHC or LCTHC) you have to use a custom Macro to do that in MACH. We have an M101 and M102 in our macros that does that function. It has to be embedded in the G-code a the right spot. The easiest way is to group the cuts that are without THC together in SheetCAM and put in the Macros or to modify the POST so you can do it atuomatically. You could tie it to a toolnumber so selecting that plasma tool to cut with would mean don't use the THC.

[WSS]

Tom, is there a spot in mach or sheetcam to specify "no thc" if the cut path is under x.xx" (user specified)? for instance turn off thc if path is under 3.14" (a 1" hole or under)?

WSS

[Torchhead]

The process of building a cut file in your CAM program should allow you to totally define HOW you want it cut. The CAM needs to know it's running a plasma job and let you specify and control the process. You can group cuts together and cut them differently than others so you can just group all of the smaller holes together, define them as a separate operation and do a different kind of cut. Example:typically inside cuts are done counter clockwise while outside cuts are done clockwise. Smaller holes need to be cut (much) slower and may even need a different lead-in style. You can modify the POST (has an open scripting language) to do just about anything you want. The scriber post is an example. It uses toolnumber to swap over to the scriber and automatically apply the programmed offsets

You can set a number in MACH (Anti Dive) that will lock the THC off if feedrate drops below a preset percentage but you have to dink with it and remember to turn it off on a lot of cuts. Our Anti-dive in the DTHC will keep the torch from diving if the voltage spikes from cutting too slow (as happens on a small hole)

In SheetCAm you have access to variables like the total length of a cut and it's used to determine how often the touch -off occurs by measuring the toolpath length (X + Y) in each cut (between pierces). You can read a tool number and make it do something totally different for that tool. You can mix tools in a job so you can scribe parts and plasma cut in the same run.

The Macros I posted when inserted in the G-code (either by the user or through the POST in sheetCAM is the same as turning the THC ON/OFF with the screen button.

There are multiple ways to make the machine do EXACTLY what you want. Doing a parameter based on just a distance is dangerous for THC control. Doing it by the type object you are cutting in the CAM is cleaner and works well