hole quality

[dsanford55]

i can't seem to find the the answer to my question searching thru the boards, so I'll ask.

I've got a HP 85 & LDR Motions, and running CNC Command software using sheetcam, cutting 3/8" plate at 19 in per min & 65 amps for the holes.
However I can't seem to get a good quality of cut for my holes.

Using a .375 lead in from the center, brand new consumables, and factory recommended settings from Hypertherm for 3/8" plate.

holes are somewhat beveled and not as round as should be.

any suggestions would be appreciated,
THANKS!!!!

[mdwalker]

Cut your holes at 60% of cut speed and see if that helps.

[mdwalker]

Another thing that can cause this is your torch height. Need to measure your actual cut height and see if it is accurate.

[jimcolt]

Email me directly and I will send the presentation called "Best Practices for Plasma Hole Cutting. There are a lot of techniques. jim.colt@hypertherm.com Keep in mind that you are using an air plasma cutter, not one of the liquid cooled, oxygen, high definition plasma's that can cut taper free, divot free holes on steel. They cost about 10x more than an air plasma....however save a lot of aggravation in secondary work. Here is a pic with top and bottom dimensions for different holes sizes cut in 1/4" steel with a Powermax air plasma:

dimensions.jpg (106.35 KiB) Viewed 2049 times

dimensions.jpg (106.35 KiB) Viewed 2049 times

[dhelfter]

The presentation Jim Colt is speaking of is actually on your computer we supplied under the manuals/cut quality folder.

Thanks
Dan
LDR

[tcaudle]

Once holes get small you need to cut them with the DTHCoff. How to do that? open SheetCMA and you will see in the OPERATION an input box named" Min Cut Length for DTHC" with a default of 1". That means it will automatically keep the DTHC from turning on at the beginning of the cut if the total lenght is LESS than 1". That only covers a hole of less than 3/8" diameter. I suggest you raise that to 3 io catch a circle of arounfd 1" diameter and below. DO NOT try to control the DTHC on/off at the beginning with a Cut rule....It won't work because the OFF run happens before the ON command and it turns it on anyway. When you slow down a cut your torch volts goes up. When you torch volts goes up the DTHC moves the torch DOWN to lower it back to the preset volts (dives) to stop that use the method above. Slowing down, picking the right leadin and turning off the DTHC on smaller holes will lead to better results. Make sure your touch off sequence is correct and the pierce height and cut height defined in the G-Code are actually being used at the torch.

[dsanford55]

appreciate all the responses fellows...thx again

[dsanford55]

Email me directly and I will send the presentation called "Best Practices for Plasma Hole Cutting. There are a lot of techniques. jim.colt@hypertherm.com Keep in mind that you are using an air plasma cutter, not one of the liquid cooled, oxygen, high definition plasma's that can cut taper free, divot free holes on steel. They cost about 10x more than an air plasma....however save a lot of aggravation in secondary work. Here is a pic with top and bottom dimensions for different holes sizes cut in 1/4" steel with a Powermax air plasma:

dimensions.jpg

Jim,
Been a few days since I posted... found the presentation you're referring to, thx

I'm going to draw some different sized holes for testing on the 3/8" and spend some time tweeking this pupy.
Thx again

[dsanford55]

The presentation Jim Colt is speaking of is actually on your computer we supplied under the manuals/cut quality folder.

Thanks
Dan
LDR

Thanks Dan... you have all the bases covered as usual, just have to look in the right place...LOL
Thanks Dan!

David

[BensPlasmaAu]

Once holes get small you need to cut them with the DTHCoff. How to do that? open SheetCMA and you will see in the OPERATION an input box named" Min Cut Length for DTHC" with a default of 1". That means it will automatically keep the DTHC from turning on at the beginning of the cut if the total lenght is LESS than 1". That only covers a hole of less than 3/8" diameter. I suggest you raise that to 3 io catch a circle of arounfd 1" diameter and below. DO NOT try to control the DTHC on/off at the beginning with a Cut rule....It won't work because the OFF run happens before the ON command and it turns it on anyway. When you slow down a cut your torch volts goes up. When you torch volts goes up the DTHC moves the torch DOWN to lower it back to the preset volts (dives) to stop that use the method above. Slowing down, picking the right leadin and turning off the DTHC on smaller holes will lead to better results. Make sure your touch off sequence is correct and the pierce height and cut height defined in the G-Code are actually being used at the torch.

A great tip Tom! I will also give this a go and see how things go.

[dsanford55]

Once holes get small you need to cut them with the DTHCoff. How to do that? open SheetCMA and you will see in the OPERATION an input box named" Min Cut Length for DTHC" with a default of 1". That means it will automatically keep the DTHC from turning on at the beginning of the cut if the total lenght is LESS than 1". That only covers a hole of less than 3/8" diameter. I suggest you raise that to 3 io catch a circle of arounfd 1" diameter and below. DO NOT try to control the DTHC on/off at the beginning with a Cut rule....It won't work because the OFF run happens before the ON command and it turns it on anyway. When you slow down a cut your torch volts goes up. When you torch volts goes up the DTHC moves the torch DOWN to lower it back to the preset volts (dives) to stop that use the method above. Slowing down, picking the right leadin and turning off the DTHC on smaller holes will lead to better results. Make sure your touch off sequence is correct and the pierce height and cut height defined in the G-Code are actually being used at the torch.

I appreciate your input seems I should be able to tweek these even better, not sure.
The pics are viewing the top and bottom sides.
The top doesn't look bad at all and would work fine, the problem is the underside. I'm getting a divot for some reason.

SheetCam and commandCNC

How can I improve on these 17/32" holes in 1/4" plate ?
Any suggestions?

inside offset operation:
" Min Cut Length for DTHC" (6)

45 AMP cut settings

A) 60% decreased cutting speed for 1/4" plate
B) lead in: .375 perpendicular (default center cut setting for circles less than 1")
C) over cut: .2
D) NO lead out


outside offset operation:
" Min Cut Length for DTHC" (6)
45 AMP cut settings
A) 1/4" 45 AMP
B) lead in: .375 (default center cut setting for circles less than 1")
C) over cut: .2
D) NO lead out

[motoguy]

I found the best, most reliable method for cutting small holes was to put the holes on their own layer. Then disable THC for that layer, and manually set the cut speed for that layer (30,40,50,60% of book speed, depending on what you're trying to accomplish).

[dsanford55]

I found the best, most reliable method for cutting small holes was to put the holes on their own layer. Then disable THC for that layer, and manually set the cut speed for that layer (30,40,50,60% of book speed, depending on what you're trying to accomplish).

thx for the reply.
I've got the holes on their own layer, so that's covered. And the THC for that operation is set in SheetCam, so that's covered. These were cut @ 60% of book speed so I think I'll try backing that down to 50% on the next series of cuts and see what taht does.
Thx!

[motoguy]

I have also gotten away from a big overcut. I used to Arc in an arc out. Now I come in perpendicular, and have about a kerf sized over cut. .06 or so on 1/4". That is not much of an over cut, but combined with the slower travel speed, it seems to clean the whole up nicely without leaving an out of round shape where the / cut digs into the edge.

[dsanford55]

I have also gotten away from a big overcut. I used to Arc in an arc out. Now I come in perpendicular, and have about a kerf sized over cut. .06 or so on 1/4". That is not much of an over cut, but combined with the slower travel speed, it seems to clean the whole up nicely without leaving an out of round shape where the / cut digs into the edge.

I think decreasing my overcut is a good idea. Looking at these pcs. when I cleaned them up the problem area was in the same place on each of the pcs. Seems when using the perpendicular lead in, when the torch starts it's cut on the radius, there's a divot. Leads me to think reducing the cut speed back to 50% or less will probably solve the issue.
This machine is just fascinating, I love it, just a learning curve. LOL

[dsanford55]

sitting here drinking coffee and surfing through these threads also discovered I'm using the wrong nozzle for 1/4" 45 Amp cutting operation.
Jim has some terrific posts and pics, discovered this on another thread.
Going to order some 220941 nozzles, looks like thats part of the problem too.