16ga woes.. need help with getting a clean cut

CrossFire ® PRO
21

I have two would like to keep one though. I don’t mind mailing you the other.

1 Like
22

All good. I have to go into town tomorrow and pick up a shut-off valve for my system anyhow. Thank you for the offer though! This community continues to shine!

2 Likes
23

Well I shine alright. Like a burnt out lightbulb!
I understand the offer stands if you change your mind.

2 Likes
24

Don’t use lead out when cutting signs with letters, get better outcome in appearance.

3 Likes
25

I would also add to put a motorguard dryer right before the plasma. that’ll get most of the moisture left in the line after the refrigerated dryer. you can get a kit that comes with 2-3 extra filters for around $100.

2 Likes
26

And in addition to @nicaDd suggestion, this advice/tip seemed good. (I can’t remember who said this, it could have been @OldNBroken)

But they said they have a pressure gauge before and after the motorguard filter. When you see a significant difference/drop in pressure on the downstream gauge, when air is being used, you will know the filter needs to be replaced.

2 Likes
27

why is your cut speed so slow? 16ga cut speed on a hypertherm 45xp is 250-320 IPM your at 90, seems way too slow. i know its not a hypertherm but its still way too slow.

28

@Dirty_Bill I kept slowing it down because of the issues I was having with the cuts not finishing, I was getting better results with a slower speed. I have the amperage set to 35. I’m all ears though and willing to try what is suggested.

29

try speeding it up. the slower you go the more heat that is transferred to the work piece.

1 Like
30

Thank you @Dirty_Bill

32

I agree with most of the feedback you’ve received here. I also run 16 gauge material, and thinner material in general, at high feedrate / high amperage. Try dialing the amperage up to 40-45A, and feedrate to the ballpark of 130-150 IPM. You can use the feedrate override in FireControl in the short term to get an idea of what a good feedrate setting would be for your G-code once you are ready to go back into SheetCAM to edit that value.

I’d also be curious to know whether or not pierce height and cut height settings are true on the machine- is that something you’ve already checked with a feeler gauge or a shim?

3 Likes
33

@langmuir-aksel how do I check the actual cut hight w/o the torch running?

34

Try running one of your G-codes in FireControl as a dry run, which will simulate the full toolpath on the machine without actually firing the torch. To check pierce height, pause the code immediately after the IHS sequence is complete, just before the torch begins to move during a cut loop. To check the cut height, let the code run the cut loop for at least half an inch after the IHS sequence, then pause.

EDIT: Should have mentioned, the dry run feature of FireControl is located immediately above the feedrate override.

1 Like
35

Ok, I might have another issue then, When I dry run the torch height stays at where I left it… the z doesn’t change and the torch just runs around in the pattern.

36

That may be my memory failing me then, dry run might actually exclude IHS sequences- I’ll need to try this on my end to verify, I haven’t personally had to do a dry run since installing the limit switches on my CrossFire.

2 Likes
37

IHS is disabled when you select dry run, there is a program posted in this forum by a member that you can run to check actual torch height. Or you can do a straight line cut and hit pause once torch starts cutting. .

4 Likes
38

Run this gcode file from @Phillipw
cut height test.tap (224 Bytes)

It will go thru the IHS (initial height sensing) and then go to the cut height of 0.060 inches and stop. Measure and see if you are at 0.060 inches. The torch will never fire with this code as it never gets the command to fire.

Here is what the file is:
(v1.6-sc)
G90 G94
G17
G20 (Units: Inches)
H0
G92 Z0.
G38.2 Z-5.0 F100.0
G38.4 Z0.5 F20.0
G92 Z0.0
G0 Z0.02 (IHS Backlash)
G92 Z0.0
G0 Z0.15 (Pierce Height)
G4 P0.5
G1 Z0.06 F100.0 (Cut Height)
M5 M30
(PS100)

Notice it also includes the “springback/Backlash” of 0.02 inches. If you are doing this test on 10 gauge or thicker, you really don’t need any springback so adjust accordingly. You will also notice, this gcode file does not include the M3 (turn torch on) command.

3 Likes
39

Thanks @ChelanJim ! I’ll run that today and see where things shake out.

1 Like
40

well, instead of being 0.060 it was 0.090… where do I go from here?

41

Modify your cut height and/or put in a negative value for springback to get you down to .06

4 Likes