Tricks for holes

[djreiswig]

I need to cut some 1/2" holes in 3/8" HR plate. I don't usually mess with cut rules in SheetCam, but this is a customer job and I don't really want to die grinder a bunch of holes. I've read a little on here about slowing feedrate and turning off DTHC.

What are the tricks to get good hole quality? I have the hytconnect option so I could adjust amps and air pressure on the fly. If I slow the speed do I also need to adjust the voltage to maintain cut height?

Sig has pretty much all my equipment.

[vanweld]

Jim Colt did a nice write up on cutting circles in the tech tips forum. Good information in there that helped me out a lot.

[Euclid933]

Have a search for Jim Colt's information on cutting Holes, or I think there is some information on the Hypertherm Web site, if I remember.
It improved my cutting of cutting bolt holes, even with my ancient Hypertherm Max100.
I have set simple cutting rules in SheetCam and I never really change or disable them, just use them on all jobs.

[djreiswig]

Care to post your cutting rules?

[vanweld]

I am still very new to the game and don't use SheetCam so I can't help there. For my setup, I followed the guidelines in Jim's post. THC off especially on smaller diameter, make sure cut direction is correct, ended up seeing best results on 1/4" at about 45% of book feed rate. I basically spent a couple hours making swiss cheese out of some plate using different settings to come up with the best result.

[djreiswig]

I guess with thc off the volts don't matter.

[Rustynuts]

I learned by watching this video...

https://www.youtube.com/watch?v=hC_TRbmlzpE&t=305s

[SeanP]

I get fairly decent holes using these setting for base plates (3000 various sizes 10mm & 12mm over last 12 months!)
I used to be die grinding but don't touch them now.
There's a lot that can be done with the cut rules, the torch off before end is very good to dial out the edge burn or whatever its called
If you have problems with parts not dropping out - tag crossing over leadin, that little slowdown at the end cures that, you sometimes have to play around to get it just on the right spot.

You don't need thc turning on for anything less than 40mm dia and definitely when slowing feedrate, just asking for bother

Hole settings for base plates

Outside cut settings for base plates.

[SeanP]

Sorry just realised I didn't have right post loaded on house computer for screenshots above, min cut length for DTHC is missing, that disables DTHC on any cut less than 200mm long in this case.

Min cut.png (52.75 KiB) Viewed 4616 times

Min cut.png (52.75 KiB) Viewed 4616 times

[djreiswig]

Thanks. I'll give those a shot. I notice in the first pic you have a torch off rule 0mm before end. Is this how you implement the early torch off?
I played with the m11/m10 in Mach a little, but haven't charted the times needed to get the cut to finish at the proper place for it to cut all the way but avoid the divot.
I'm going to play around with the holes this weekend, so we will see how it goes.

[SeanP]

Yes it ranges for thicker materials 10mm & 12mm turn off 0mm before end to 2.25mm before end on 3mm using 45a parts on my machine, and that's un - ticking 'include leadout'

Finecuts seem a bit more finicky at getting just the right spot, you can stop that burn mark when the slug drops in a lot of cases.

I had a massive job over Christmas 14off 1.25m x 2.5m sheets of 2mm riddled with 25mm holes, some 23,000 in total I did struggle to be honest either getting rid of the burn or not having the centre fall or leaving a little tag left by, so ended up settling for decent hole and a slight burn as it dropped, ran over the whole sheet with a ceramic 80 grit then ran over with the knotted brush to smooth the edges, it worked out well, sheets kept nice and flat, 2.5hrs a piece to cut though,,, I would do them again though no probs €€

[djreiswig]

So you have different rules to turn the torch off early for different thicknesses?

[SeanP]

Yes I do, best way I have found so far is to save each material as a separate toolset and load that.
Seems to wok ok.

[djreiswig]

Do you use the M11/M10 in Mach or just the cut rules with SheetCam putting in the M5 early?

[SeanP]

M10
It's does have P1 after it as well not sure if it makes any difference

[djreiswig]

I think you need the P1 but you set the output in the Mach settings so it doesn't actually do anything.

[robertspark]

Note.... That minimum cut length for DTHC is a custom field added to sheet cam by the selected post processor

M11/M10 is another animal.....

M11 (in mach3) turns the output ON and M10 turns the torch off (some software works the other way around... Like uccnc)... M62/M63 are the equivalent codes in mach4 and linuxcnc

In order to use M11/M10... M3 had to first be active. In mach3 M11 will only be active while the machine is moving / in motion..... If the machine stops the m11/M10 defined output will go off.... Whilst this may not be obvious.... If you toggle any other M (miscellaneous) code during a cut the machine will stop whilst executing that m code.....

M10/M11 in mach3 was a laser power / enable signal and it's purpose was to fire a laser to cut / mark material in sync with motion.... If motion stops.... The output stops... When motion resumes.... The output resumes....

So.... Say you enable and disable THC in mach3 with a custom miscellaneous (m) code.... M222/m223

Every time you toggle those codes during the cut.... Motion will stop whilst they are being executed.... This will be seen as a slowdown in motion....
Try it ....... Get two linear G1 moves... Say (assuming your machine is in inches), create a *.tap file and type in it
G64 (constant velocity)
G90 (absolute distance mode)
G92 X0
G1 X15 F200
G1 X30

Now create a second file

G64 (constant velocity)
G90 (absolute distance mode)
G92 X0
G1 X15 F200
M234
G1 X30

What motion controller are you using????
Parallel port, ESS or something else

[djreiswig]

ESS

[robertspark]

ESS the M11 px number does not make any difference as you can only have 1 M11 output.

Originally.... When M11 was created .... It was created for the parallel port and you could have a few ports which toggled via M11 P1, M11 P2 etc....

Check the ess plugin as that is where you define your one and only M11/M10 output.

I got rid of my ess a short while ago.... Been gathering dust for 2+ years now...

..... Shameless plug.... Again.... We can define a load of M10/M11 pins in uccnc.... And we have dedicated macros for thc which operate in sync with motion (or toggling the THC on and off has no slowdown or hesitation.... Because the m-codes operate in sync with the motion.... (Nope I don't work for cncdrive or recieve any kickback... Just saying there is another way....)

[djreiswig]

Okay. Thanks for the info.

[see&see]

Here's a copy of Jim Colts presentation for cutting holes posted publicly in several places..

[Tautog13]

see&see
Thanks for Jim Colts .pdf

C

[jimcolt]

Your welcome! Jim Colt

[djreiswig]

I experimented this weekend and ended up oversizing my .5" holes to .505 and slowing down feedrate to 30%. I tried slower, but the holes seemed slightly out of round. Not much dross, and a small amount of die grinder work and the bolts fit snug. Much better results than at full speed. Thanks for the help everyone.

[Euclid933]

My cutting rules are a little like SeanP, except I don't have AVC on my machine, just a plate runner.
I tried the Anti-spatter spray on some 10mm plate yesterday. It seemed to work well on my machine.
It reduced the amount of dross on the top of the plate around the pierce, which is very useful with a plate runner setup like mine. The plate runner can sometimes bump over the dross and affect the cut.
The added bonus is it smells like a Fish and Chip shop.
Good look with getting it setup.
Will.