[DISCONNECTED]

USING SHEETCAM WHAT KIND OF PIERCE DELAY AND PLUNGE RATES ARE A GOOD STARTING POINT FOR PLASMA CUTTING.USING CandCNC THC.

[Apples]

Go to the manufacturers website of the plasma and look for the pierce delay, cut speeds and pierce height info there

[Torchhead]

You do not need a hard pierce delay except on material thicker than 3/8" (depending on the plasma unit and tips being used) if you use the Arc Good signal (required on the MP1000-THC). It automatically sets a variable delay based on the conditions. Using a manual delay means you have to set it for worst case (purge air off) so needs to be longer on some pierces that it should (which causes other problems). Typical delay with a hot torch and purge air on is about .5 sec for material of 1/4 or less. For 1/16 it's almost instantaneous. Some THC's require you to set the pierce delay as a number and change it for every type of tip and material. Using the Arc Good approach where MACH holds movement until it gets a signal there is a valid pierce works a lot better and keeps the XY from taking off if you have a condition where you lose arc.

Plug rate is just the speed at which to move from initial pierce height (set in SheetCAM) to your initial cut height (set in SheetCAM) occurs. The distance is typically less than .1 inch. I typically plunge at about 1/2 to 2/3's the max velocity of my Z axis or about 40 IPM. It's a good idea to put in a hard 1 sec delay at the end of cut (also in SheetCAM)

The cut charts will not ususally give you the pierce height but the general rule is to pierce as high as you can and still get a clean pierce. The Hypertherm tables of feeds and tip volts is based on maintaining 1/16" cut gap. I typically pierce at 1/8" or slightly higher. The higher pierceing keeps blow back of molten metal (which goes out in a crown shape as you pierce the metal) from clogging the tip. Clogged tips short out and shorten their life considerably (or instantly!)


I have several plasma "tools" defined in SheetCAM for different tips and material. Kerf offset numbers for my machine worked out to be roughly equal to the tip cut current. (i.e. 40A tip has about a .040 (actually 048) kerf width.

Also there is a Chart in MACH3 for the MP1000 that will let you define and select the target tip volts for a given material and send it to the MP1000.

Other help on cutting and setup are available over on the CandCNCSupport Yahoo group where we answer all kinds of questions about how to use our products.

Tom Caudle
www.CandCNC.com

[Dale Heart]

I just saw how some Japanese pierce their material. All I can say is that I've never seen a torch move up and down so much and also have never seen a cleaner pierce in my life.