reaming out holes

[speedmetal75]

what are you guys using to drill out plasma cut holes? i tried using a regular drill but it seems to mess them up

[Torchmate]

I will hit my guys up in the morning when the shop opens up. Jesse might be on here before then with an answer I suspect.

[StinkBug]

It really depends on how much undersize your holes are. If they are really close to the finished size then you'll tend to chip the corners off your drill bit. If you have the TM cut them a bit smaller it's not as hard on the bit. Generally I cut my 5/8" holes at 9/16, my 9/16 at 1/2, etc. The plasma cut edge is a bit hard on bits, but it's not too bad. I just use the cheapie HF bit sets and replace them every couple months. Everyone around here likes to abuse bits anyways, so it's not worth buying the expensive ones.

[Arya Ebrahimi]

A related question I've been wondering is how accurate is the plate marker? Could you lay out say a bolt pattern with the plate marker and then drill the holes with a drill press? I'm curious what kind of tolerances you could hold with this system of locating/drilling holes. Would it be more accurate to do it as I've described or to "finish drill" holes cut by the plasma?

[abrogate]

It is surprising how many people are having issues with this. I never knew that this was such an issue before I bought my machine. I tend to break the edges of every drill bit I try to put through the plasma cut hole. It is a bummer that this sub-forum wasn't around when I bought the unit, otherwise I would have probably spent my money differently.

As far as the holes go, I don't have the plate marker yet, but I plan on getting it soon. I am going to mark the items and drill the holes with an annular cutter. Some holes can't be drilled with a press, so I ended up buying a mag drill (check eBay) and I hope that this makes my days a little less frustrating.

[bogger44]

Again not a tm but on my table I put a mark in the center of the hole so it just makes a pierice point then I drill out with a 1/4" good quality bit then drill from there. Works real good .because of the air plasma it nitrates the surface and case hardenes it that's why it reacts like that.

[jimcolt]

Air plasma cutters produce a nitride (about .005" thick) finishe on carbon steel...this is a chemical hardeneing that will destroy drill bits and reamers quickly.

It is best to use a good quality plasma system that is dialed in correctly to produce holes that require little or no rework...not all air plasma systems have adequate arc energy density to do this.....if it is a Hypertherm system I can often help you get it dialed in for good holes.

Improving holes:

1. Use the smallest nozzle and process power level for the material you are cutting. If cutting 1/4" steel and you want some nice 3/8" holes.....an 80 amp process will not work....it will provide a severe taper. Use a 40 amp process.
2. design the hole lead in to pierce in the center of the hole....ensure adequate pierce delay, and ensure that your pierce height is 1.5 to 2 times the manufacturers (plasma torch) recommended cut height. If you have a machine with excellent acceleration (in excess of 40 miligees) and your machine is mechanically tight (no backlash or flex)...then a straight lead in design is best. If the machine is sluggish or has backlash...use a radial lead in. the plasma process likes to cross the lead in kerf at a 90 degree angle.....but backlash and sluggish acceleration will cause a divot in the hole....so revert to a radial lead in if needed.
3. Ensure that as soon as the pierce is complete...that the THC indexes the torch down to the cut height.....while the arc is still on the lead in kerf. The torch needs to be at proper cut height before it gets on the hole profile.
4. Program hole speeds on all holes under 1-1/4" diameter...to cut at 60% of the speed you are cutting the outside parts contour at....this is to help minimize the taper.
5. At the end of the hole.....do not use a lead out that goes to the center of the hole, rather, if your software allows it, design an overburn of .200"...this is simply an extension of the hole radius past 360 degrees. If your system has the capability (some machines don't)....issue the plasma off signal at exactly the 360 degree point of the hole.....and the overburn should keep the motion goig while the plasma is extinguishing. (plasma systems do not shut off instantly on steel..there is an exothermic reaction that takes a few miliseconds to shut down...and this can leave a divot in a hole profile.....by continuing movement, the divot is minimized).
5. Also....on holes (rule of thumb) under 1-1/4"....the THC sould be frozen at cut height.....the AVC (arc voltage control) should be disabled.

I have pics of a piece of 3/8" steel cut with a Hypertherm Powermax45 with 3/8", 1/2", and 3/4" holes that require no rework.....there is very little taper and bolts pass through just fine. For some reason this site won't alow me to post pics.....

If you cannot get good holes with your equipment.....make your holes all 1/2 size in your program.....and then drill them out with a high quality drill of the correct size.....good drills cost more...and they are woth every penny. By making the holes much smaller, you are cutting the hardened material with an inner cutting edge of the drill as opposed to putting the stress on the outer edge...which chips easily.

Jim Colt Hypertherm

[MQYJ]

For any holes that need to be accurate, I have found that it is easiest on drill bits and much less frustrating if I layout hole centers with the plate marker and then drill the entire hole. If I was doing big runs of parts with holes I would either spend the time to get my machine dialed in perfectly or find a different process to cut parts all together. It also has been said on here before that Plasma is not necessarily the best process for creating perfect holes every time.

[jimcolt]

Air plasmas do not do perfect holes by themselves. It takes good coordination of programming (lead in, lead out, cut speed) , torch height control, machine motion, and plasma process control. Very nice holes are achievable with plasma using the correct techniques.....as long as you have the right equipment!

I have a .pdf presentation on best practices for hole cutting that I will forwar to anyone interested....just send me a note to my direct email jim.colt@hypertherm.com and I will forward it to you.

Jim

[HardcorewannabeXJ]

On the holes that we need to be just the right size, we usually cut them slightly undersized (maybe .015 to .020") and then send a drill bit through. Most of our holes are simply cut to be the correct size so that you don't need to drill them afterwards.

What I experience from most customers is that when they are cutting say a half inch hole, they can't fit a half inch bolt through. This isn't necessarily a Plasma cutter or Machine problem (although it can be) but a programming problem. When you are doing a toolpath in the Torchmate CAD software there is a Kerf Width value that can be set in order to produce as accurate as possible cuts. Cutting 40 amps through 12 ga material will give you a different kerf width than 80 amps through .25" material. The only way to know exactly the amount you need the software to adjust for is a matter of cutting a straight line in that material at your appropriate cut speed, and take a pair of calipers to it. The top of the cut will be slightly smaller as the bevel usually angles outward on the cut. So if you are trying to fit a bolt through a hole, you would want to know the bottom value.

Also a few customers on non-critical bolt holes oversize the holes .015"+ when drawing before the toolpath, to keep themselves from having to drill anything out. It's all a matter of what you want to do.

The procedures mentioned by Jim are going to help improve your circular cut quality every time, so I would recommend following them. I believe the Torchmate CAD Users guide goes into this in brief detail as well.

In the end, some people are in search of a perfect hole that can only be achieved by drilling or punching them out afterwards, and I would suggest either using the machine to mark a pilot hole or mark with the plate marker a point as to which the hole needs to be in order to save you the time of laying out the holes afterwards.

In response to Arya's question, the plate marker is accurate to about .01" and has a marking width of about .03". In regards to marking a pilot location, via either a pierce hole or with the plate marker, you can do it either way. The holes location however will be determined more by the person doing the drilling. Plasma pierce holes are not perfectly circular around the center of the torch body, so drilling them can sometimes be a pain if the drill wanders off center when you are starting to drill it. Plate marking can give you a pretty serious center point that "should" hold the drill on center and allow you to drill it out, but there is still a chance it will wander.

[Rocco]

Just a tip for drilling. If you put a flat on the face of the cutting edge the drill will last longer and not chip as easily.

[waynehartwig]

So question on this:

1. Use the smallest nozzle and process power level for the material you are cutting. If cutting 1/4" steel and you want some nice 3/8" holes.....an 80 amp process will not work....it will provide a severe taper. Use a 40 amp process.

So do you then cut everything at 40A? Or do you just do your holes, then come back with 80A to cut the part out?

[jimcolt]

The best quality with plasma is always with lower power, smaller orifice, but of course enough power to cut with minimal dross.......so if I wanted the best quality on the entire part....I would do it all at the same amperage......if I wanted to cut the outside contours at higher speed, with a bit more edge angularity...then I suppose I would switch to a higher current, larger nozzle orifice.

Other metal cutting processes (water jet and laser) use similar techniques to get best quality on small features......you cannot expect good quality on thin material with a laser at 6 kW output....just does not work well!

Jim Colt

[StinkBug]

Originally Posted by waynehartwig

So question on this:


So do you then cut everything at 40A? Or do you just do your holes, then come back with 80A to cut the part out?

I generally cut everything with the lowest amperage that will make a clean cut. Running at 80A may allow you to run faster feedrates, but generally I'm more concerned with making clean accurate parts than saving 30seconds of cut time. If I were cutting hundreds of those parts it might be different, but I'm not.

[waynehartwig]

Makes sense Still learning over here...

[jimcolt]

Another comment from me....I like locating my holes with the plasma.....and getting them right by using good techniques.....however if you have to locate your holes with plasma and then drill or ream them......you can be assured that they are in the right location...as the holes were all located with the same TCP (tool center point). When using a device such as a scribe...that is offset from the torch.....then your torch contours and scribe markes are accurate only if the scribe is in the exact correct location. I have seen many offset marking devices that caused tolerance issues on the plate...usually because the opertor bumped the marker (or the plasma torch) and either forgot to reset the correct offsets.....or measured incorrectly.

Hypertherms HPR (high definition class plasma) can mark (called arc writing) and cut using the same nozzle orifice...marking is done with argon for no hardening of the plate.

Jim Colt

[MQYJ]

Those of you laying out a hole center with a plate marker, how are you drawing the hole center in CAD?

a single node? a cross hair?

[HardcorewannabeXJ]

Originally Posted by MQYJ

Those of you laying out a hole center with a plate marker, how are you drawing the hole center in CAD?

a single node? a cross hair?

It depends. A small circle is the easiest. Since with the plate marking no tool-pathing is required, the machine will see a very small circle (.01") and just make a barely noticeable motion (if any) at that point. Seems like the easiest way for a simple bolt hole location.