mach 3 status no tool

[acourtjester]

To fire the hypertherm it requires only the controller to close contacts, if you take the 2 wires for the Hypertherm and touch them together it will fire the torch. The THC should not be firing the torch, the THC only requires the arc voltage output from the Hypertherm. That is used to tell the to move up or down depending on the set voltage level. The torch fire circuit is an totally different signal path not in the THC. You need to change the trigger signal for the relay that is firing the torch. Find the signal to the M3 in the G-code or F5 keyboard in Mach 3 that is what should be triggering the relay.

[NB Forrest]

Tool 1.png (36.94 KiB) Viewed 1617 times

Tool 1.png (36.94 KiB) Viewed 1617 times

Almost there! My torch works! It turns on and off at the proper place. However I have to have the THC button turned off and my torch rides about an inch over the plate. I'm using SheetCam and my tool settings are shown. Why would my torch not follow the SheetCam G-code? Is there a setting in Mach3 I don't know about? I'm not sure my THC is working properly is why I am taking it out of the equation and just trying to get everything functional then I will address the THC. This is a great fourm, I don't think I could have gotten this far without y'all.

[acourtjester]

Your SheetCam tool is correct, how are you showing the metal surface for the G-code to follow?? You need to use either a floating head switch or Ohmic sensor which tell the controller where to start from. For a test you may set the torch touching the metal surface and run this G-code no Plasma. If it functions without plasma then turn on the plasma on to for a complete test. It is only running at 40 inches per minute so it will have dross. You can change the F value from 40 to higher for on the line 6 like 48 for 1/4" steel.
This G-code should move the torch up to 0.160" fire the torch and cut a square 2" X 2" and turn the torch off.
G92 Z0.0
G00 Z0.1600
M03
G04 P0.5
G01 Z0.0600 F3.937
G1 X2.00f40
G1 Y2.00
G1 X0.0
G1 Y0.0
m5 m30

[NB Forrest]

I'm not sure I understand. you said ", how are you showing the metal surface for the G-code to follow?? " I'm not sure what a floating head switch is or an ohmic sensor. I do have a THC but I have it disabled until I have this working. Also how do you know it is running at 40 ipm? I thought it was running at 200 ipm because that is what I have set it at, or I thought so.

[acourtjester]

Ok I know these thing are new to you, as it was with all of us, so I will give you a quick overview. The attached video shows how the torch moves to find the metal surface with an ohmic sensor, it is similar as it works with a floating head switch. The THC is a completely separate operation but it does happen after the metal surface is found so thinking they are related is normal. When a cut operation is planned and the G-code is generated a Post Processor is used in SheetCam. There are all kinds of post processors in SheetCam that are related to the controllers electronics and software.
In the post processor things like how to find the metal surface, what the cut and pierce height are, speed of the torch travel, ect. For testing I said move the torch down to the metal surface, just touching it. Then run the short G-code is typed in above, it is very simple. The G92 tells the controller to set the Z DRO to 0.0 the staring point for that G-code. It will then move the torch up to 0.160" (pierce height) then fire the torch. The G04 po.5 is a delay for the plasma to cut through the metal. Next is to move the torch to cut height at 0.060", next move the torch X 2" then Y 2" then X to 0.0 then Y to 0.0 and turn off the torch. In other words cut a 2" square at a speed of 40 inches per minute. First with no plasma to see the action, then with plasma on to see if it will cut metal. If that works the rest is learning how to create your own G-codes and use either a Ohmic sensor or floating head switch. One step at a time.

[adbuch]

I'm not sure I understand. you said ", how are you showing the metal surface for the G-code to follow?? " I'm not sure what a floating head switch is or an ohmic sensor. I do have a THC but I have it disabled until I have this working. Also how do you know it is running at 40 ipm? I thought it was running at 200 ipm because that is what I have set it at, or I thought so.

Tom gives a great explanation about the difference between firing the torch and thc (torch height control) which monitors the divided arc voltage and attempts to maintain a constant cutting height (torch to material distance) by raising or lowering the torch using a closed feedback loop. If you have your thc disabled, then you will need to manually set your cutting height distance by physically measuring the distance between the torch and the material when the machine is cutting.

Draw a straight line about 12" long, command your table to cut this straight line, pause partway along the cut path and physically measure the actual cut height. If it is not correct, then adjust your software specified cut height and repeat until you are cutting at the correct height. For my Hypertherm cutters, this would be 0.060".

I don't personally use Mach3 for plasma cutting, but I do use it with one of my cnc routers and for that application, I manually zero out the Z axis cutting bit to the surface of the material being cut. If I were running a plasma cutter on my Mach3 table, I would move the Z axis down until the torch nozzle is 0.060" above the material to be cut, then hit the Zero button in the Mach3 screen for the Z-axis.

If you are not running your thc, then you will want to make sure that your plasma table is flat and that it is parallel to the XY plane of motion for the table. Otherwise you may have problems with your cut height either too high or too low and possibly running the torch into the material.

David

[tcaudle]

Let me shorten the answer about the THC, the touch off, and the incompatibility:

You need to remove that THC, It WILL NOT work . Pried. Toss it, Sell it, hide it use it for wall art....just don't try to use it on that table!

The whole touch off and manual cut process is 100% G-code. All you can do is move the Z down using a A G28.1 call in code and then have code Zero the Z DROo. Then you apply the "switch offset" (distance the Z overruns before tripping the switch below zero) You move the Z back up that amount then Zero the Z Again. That makes the top of material Z zero and changes it on every touch off. It has too be in the code before every pierce. Its called IH'S (initial Height sensing), Is NOT part of the THC in most circumstances.

The key is the G28.1 call that tells it its a touch off move rather than just a G0 type move.
Upi have to add hard values into the POST For SwitchOffset.

IF and when you get a THC that WILL work withy he Pokeys then your POST and INS will change.