Kerf

[JAH]

Would lowering my kerf size help when cutting the fine detail in the art work.

[beefy]

How would you make your torch cut a narrower kerf.

If anything, when cutting fine detail, where you have lots of direction changes and heat build up concentrated in one area, then due to torch slow down (acceleration & deceleration), you can end up having wider kerf width.

So simply setting a lower kerf width in your cam software does not actually make the torch cut a narrower kerf in the metal. The kerf width setting in your cam software is used to simply offset the torch by half the ACTUAL kerf width so the part comes out the correct size.

The best bet you have is using the smallest nozzle that can do the cut.

[JAH]

I thought I had read somewhere else that adjusting the kerf value a little would help the cutting of tight radius areas that error my machine out. Thats why I was asking you fine folks cause I knew I would get the correct answer . I am locked out of the compensation settings so I cant adjust it out there. So really I am just grasping at straws.

[mdwalker]

I don't know of a way of lowering the kerf size for a specific set of consumables when your speed, power, and height settings are dialed in. You can however get better detail by making sure your kerf offset is set correctly.

[acourtjester]

The kerf value is really only used in the CAM program to give a visual display. This helps in seeing if the cutting will interfere with other parts you are cutting. IMHO

[weldguy]

Would lowering my kerf size help when cutting the fine detail in the art work.

Yes, lowering your actual kerf size will help. The only real way to do this is by using a nozzle with a smaller orifice, for example switching from a Hypertherm 65 amp nozzle to a 45 amp or Finecut nozzle will produce a narrower kerf width.

If your already using the smallest nozzle available to cut the material your working with and your kerf width is set properly for that nozzle and your still losing detail you will want to go into your CAD and adjust the design in those areas where your having trouble. This is really the only way to get it done properly and maintain correct dimensions.

If you are working on an artistic piece and fine dimensions are not a concern then yes you can simply lie to your software and say your kerf is wider than it actually is so it will adjust for that and leave more material behind.

Hope this makes sense and helps.

[beefy]

The kerf value is really only used in the CAM program to give a visual display.

Not true at all.

Yes having a visual display can be useful to see if cuts will interfere with each other etc. but that is not the primary use of the kerf setting.

The kerf value determines the torch travel path offset from the edge of the part, so that the part comes out the correct size.
To illustrate, see the attached image. This is a 40mm square and the torch has been given a kerf diameter of 2mm in the CAM software (to make figures easy).
The bottom left of the square has been placed at X0 Y0 (bottom left corner) of the material to make the kerf/torch position more obvious.
The left image shows the full kerf width of 2mm and the 2mm diameter yellow circle illustrates the torch jet itself.
The right image shows the centre of the torch travel path with the kerf width view turned off.

As can be seen the CAM software has offset the centre of torch 1mm (half the kerf width) from the part outside perimeter so that the part comes out to the required 40mm. If the kerf setting did not offset the travel path by 1mm the square would end up being 38mm instead of 40mm.

KERF WIDTH & TORCH POSITION.jpg

[acourtjester]

That is correct as long as the kerf setting is by the book for each tool the program does make the part size correct. Changing the kerf width to an incorrect value will not help to make the kerf smaller. Which is what I think the OP was talking about. Also the offset selection when doing a plan will affect the part size.

[ROKCRLER]

Excellent tech info! Thank you guys for the explanations.

[JAH]

Well what I was really trying to figure out and I think I just went the long way around it. I drive a 1.5 million dollar machine and I can't cut grass detail for example. It gives me compensation errors. I was trying to ask if changing the kerf value would work to trick the machine, since I can't change the setting itself from .003 to .001. Those numbers come from beckoff website. .... But I went ahead and tried it yesterday and it did not work either.

[weldguy]

Ok I'm confused... you have a 1.5 million dollar plasma cutting system or are you working with a different cutting process?

Sounds like you need go into your CAD and adjust your design to eliminate your problems, your system doesn't seem very flexible although for that price it should make you breakfast and give you a back rub each morning before it starts cutting.

[SRdesign]

Ok I'm confused... you have a 1.5 million dollar plasma cutting system or are you working with a different cutting process?

Sounds like you need go into your CAD and adjust your design to eliminate your problems, your system doesn't seem very flexible although for that price it should make you breakfast and give you a back rub each morning before it starts cutting.

[djreiswig]

He said he drives a 1.5 million dollar machine. I'm guessing some sort of construction or earth moving equipment. Possibly a crane or dozer?

[JAH]

It's a messer cutting machine . It has two hyperterm 400 , 4 oxyfuels and a drill spindle and the table is 170' long.

[JAH]

update... previously I just adjusted my kerf value just a little but I have found if I take it from .085 on my 80 Amp to .000 it will work with no error.