Powermax 45 holes 10mm

[SeanP]

What do you reckon, should I be able to get a lot better than this?
front face is good, just cant get rid of the lead in/out tag.

10mm thick, 32mm & 20mm dia holes, perpendicular lead in arc lead out, I have had to do a little slowdown rule for a couple of mm to catch the overlap tag on the leadout, slug drops out ok.

Did wonder about arc leadin, but that doesn't get the slag pile out of the way enough.

Consumables are new apart from the shield, its in good nick though.

Thanks for any help.

[beefy]

.

[acourtjester]

That almost looks like it started the arc lead out before the circle cutting finished. Causing a flat area on the circle I just checked SheetCam and you can enter a negative value in the over cut box but don't know if it would cut with that in the G-code.

[SeanP]

I think I do have a 1/2mm overburn in there as well, maybe I should try without any slowdown rule and try a overburn on its own.
I always seem to struggle to get anything over 8mm to fully cut at the leadout.

[SeanP]

I'll try again without this lot in the morning and just us the overburn.

[beefy]

Sean,

just a guess but maybe it's the slowdown that's making it bellow out at the end.

Will it not work to have NO leadout, no change in speed (i.e. no slowdown near the end), but try different lengths of overburn, and the biggy, turn off the torch before motion stops using the M10/11 command. I'm working on the thought that you want minimal disruption of speed, potentially caused by a leadout.

Or put another way, just have a stupidly long overburn but try different torch turn off points (disclaimer - it's all theory ).

Keith.

[SeanP]

Thanks Keith, looking a lot better this morn, ditched all those rules there and just went with a 1mm overburn and the torch off.

Underside:

[davek0974]

I hope i can get holes that good when my new table is running;)

Rules 3 and 4 seem confusing, rule 3 you slow to 60% at 3.5mm before end and rule 4 you speed up again to 100% at 2mm before end???


I often find it helps to scratch the sheet across where the circle is going to be, make the cut, rescue the slug from the pit and pop it back in with the scratch aligned - that way it helps to see exactly what is going on in the cut.

[SeanP]

I did make that rule set for another job that was giving me grief where the last part of the cut crossed over the lead in, it just seems to wander over that bit and leave a bit hanging on, I used that to slow down on that bit so then it dropped out, it has worked ok on some jobs, it's a bit of a fudge though

Rules 3 and 4 seem confusing, rule 3 you slow to 60% at 3.5mm before end and rule 4 you speed up again to 100% at 2mm before end???

[beefy]

The last few months I've had my head in books a lot, designing my own Mach3 based plasma system & THC. This journey has led me to start looking at other cnc controller softwares. Mach3 will not be for sale at some point only Mach4, a very different beast and only half working at the moment.

Talking over on the Machsupport forum, some of the lads are using UCCNC, and the one thing I'm noticing is a few of them are saying how the trajectory planner is light years ahead of Mach3. Basically the control of the motion is much smoother and accurate.

The point I'm making is I wonder if Mach3 is not always perfect with it's motion control and could this sometimes affect circles. If anyone out there has tried everything to get a nice round circle but they don't come out round, I wonder if a different PC could help. Seems to be a bit of luck finding the perfect PC for Mach.

You don't seem to have that issue Sean, your circles look great.

Keith

[Shane Warnick]

FWIW the last picture looks about as good as I can get, if the bottom of the cut is facing up (it's upside down, and the little tag is actually on the bottom after it's cut). I reduce speed to 60% of whatever I cut straight lines with, THC off, and use an overcut (negative gap at the end of the loop if you will) and 0.05 second (5 hundreths of a second) overburn, but the overburn is only on material 1/2" and thicker. I think if my guzenta's and takeaways are correct, you are cutting 3/8" steel, so I would use an overcut and no overburn on that thickness. I don't use an arc lead out (I don't think my program will even do that without a manual edit on each path) so it just recuts over where it started, after it makes the lead in and turns and starts the main path if you will. So, it leads in, comes all the way around, then continues cutting along the edge of the circle PAST the lead in cut for however long I tell it.

When playing with this as well as overburn, keep in mind that torch off doesn't mean that oxidation and actual burning of the steel stops immediately, especially when post flow is going to still be on. The thicker the material, the more molten metal there is, as well as residual heat, and I have seen metal burning on the slat (molten metal that was ejected from the kerf) for a second or two after torch off, and have watched it burn in the cut long enough afterwards to notice it (hard to time but it's happening). I think this is what makes some of the dross so damn hard where the lead in comes in and changes direction, then gets cut right up to or over again, is that it's burning and actually oxidizing some of the dross, and is really welding itself on the back side of the cut.

Regardless, I think given the process being used, that last set of circles looks better than what a lot of my competitors are getting, and I think there is a point of diminishing returns on things such as that as well. Now on 1/4" and thinner, there is zero way to tell the top from the bottom, and zero flat spot, no little tit or dimple etc. Looks damn near like it was drilled, unless it is smaller than the thickness of the plate.

Regarding height control, if the hole diameter is at least 1.5x the thickness of the plate, I will run height control and cut at 80-90% of straight line speed, and ALWAYS use it on large holes, say 2" and up diameter.

Stay safe

Shane

[SeanP]

Thanks Keith,

I'm happy enough really with the candcnc/mach3/sheetcam setup, it's the operator that falls short most of the time!!!

My biggest problem is anything over 8mm thick really, it's definitely when crossing the lead in to finish the cut, very rarely do I get parts to drop out without some sort of fudge at the end to catch that tag, I feel a powermax 65 might have been better for me really.

I think the 45 is superb on 6mm, never any problem with parts falling out there.

All 6mm below:

Topside

Underside

The last few months I've had my head in books a lot, designing my own Mach3 based plasma system & THC. This journey has led me to start looking at other cnc controller softwares. Mach3 will not be for sale at some point only Mach4, a very different beast and only half working at the moment.

Talking over on the Machsupport forum, some of the lads are using UCCNC, and the one thing I'm noticing is a few of them are saying how the trajectory planner is light years ahead of Mach3. Basically the control of the motion is much smoother and accurate.

The point I'm making is I wonder if Mach3 is not always perfect with it's motion control and could this sometimes affect circles. If anyone out there has tried everything to get a nice round circle but they don't come out round, I wonder if a different PC could help. Seems to be a bit of luck finding the perfect PC for Mach.

You don't seem to have that issue Sean, your circles look great.

Keith

[SeanP]

Thanks Shane,
Some good points there, I'm not to far away to your recommendations, I don't quite follow the overburn part though, are you using sheetcam? I only see overcut option, I mostly use the torch off rule to turn the torch off just as it gets to the lead out or very slightly before so although the machine keeps moving along the lead out the torch switched off before turning, works a treat at stopping that burnt blob on the hole edge.
I'm sure I tried not using a leadout and just having the torch off, I still got the burn mark doing that way though.
Cheers

FWIW the last picture looks about as good as I can get, if the bottom of the cut is facing up (it's upside down, and the little tag is actually on the bottom after it's cut). I reduce speed to 60% of whatever I cut straight lines with, THC off, and use an overcut (negative gap at the end of the loop if you will) and 0.05 second (5 hundreths of a second) overburn, but the overburn is only on material 1/2" and thicker. I think if my guzenta's and takeaways are correct, you are cutting 3/8" steel, so I would use an overcut and no overburn on that thickness. I don't use an arc lead out (I don't think my program will even do that without a manual edit on each path) so it just recuts over where it started, after it makes the lead in and turns and starts the main path if you will. So, it leads in, comes all the way around, then continues cutting along the edge of the circle PAST the lead in cut for however long I tell it.

When playing with this as well as overburn, keep in mind that torch off doesn't mean that oxidation and actual burning of the steel stops immediately, especially when post flow is going to still be on. The thicker the material, the more molten metal there is, as well as residual heat, and I have seen metal burning on the slat (molten metal that was ejected from the kerf) for a second or two after torch off, and have watched it burn in the cut long enough afterwards to notice it (hard to time but it's happening). I think this is what makes some of the dross so damn hard where the lead in comes in and changes direction, then gets cut right up to or over again, is that it's burning and actually oxidizing some of the dross, and is really welding itself on the back side of the cut.

Regardless, I think given the process being used, that last set of circles looks better than what a lot of my competitors are getting, and I think there is a point of diminishing returns on things such as that as well. Now on 1/4" and thinner, there is zero way to tell the top from the bottom, and zero flat spot, no little tit or dimple etc. Looks damn near like it was drilled, unless it is smaller than the thickness of the plate.

Regarding height control, if the hole diameter is at least 1.5x the thickness of the plate, I will run height control and cut at 80-90% of straight line speed, and ALWAYS use it on large holes, say 2" and up diameter.

Stay safe

Shane

[beefy]

One more tip that was told to me by a company here called ART, was to LOWER the cut height when cutting circles. Their reasoning is to use the opposite bevel to your advantage in an attempt to get less bevel in the hole.

You know how when the torch is too high the kerf is wide at the top and narrow at the bottom, like a normal "V", but when the torch is too low, it's the opposite way round and the cut flares out at the bottom like an upside down "V". Holes often have the bottom diameter much less than the top diameter so they reckon lowering your cut height for holes helps the bottom of the cut to flare out a bit and straighten up the taper. Haven't really played with it myself yet.

Sean, do you mind telling what specs your computer is, you are obviously getting excellent projectory control with your Mach3/PC combo. What motherboard model and processor are you using.

Cheers,

Keith.

[SeanP]

That doesn't seem to work on the 45 Keith, I can cut with the torch near enough touching the plate and the taper still doesn't go the opposite way, would be handy if it did do though.

My pc is a Dell Optiplex 745 small form, 3ghz, got it off ebay cheap enough so got 2

I had a similar spec machine what I started with, not a known make, it seemed ok, passed the mach 3 test fine, but I was getting a flicker doing the lamp test and at the time had quite a few missfires, the Dell near enough cured that, just get the very occasional one now.
Strange thing is the motors dont just sound quite as sweet using the Dell as they do using the the other, all settings exactly the same as far as I can see anyway, not sure what that's all about but it's not loosing steps so just ignoring it.

One more tip that was told to me by a company here called ART, was to LOWER the cut height when cutting circles. Their reasoning is to use the opposite bevel to your advantage in an attempt to get less bevel in the hole.

You know how when the torch is too high the kerf is wide at the top and narrow at the bottom, like a normal "V", but when the torch is too low, it's the opposite way round and the cut flares out at the bottom like an upside down "V". Holes often have the bottom diameter much less than the top diameter so they reckon lowering your cut height for holes helps the bottom of the cut to flare out a bit and straighten up the taper. Haven't really played with it myself yet.

Sean, do you mind telling what specs your computer is, you are obviously getting excellent projectory control with your Mach3/PC combo. What motherboard model and processor are you using.

Cheers,

Keith.

[beefy]

Thanks very much Sean,

Keith.

[Shane Warnick]

[quote="SeanP"]Thanks Shane,
Some good points there, I'm not to far away to your recommendations, I don't quite follow the overburn part though, are you using sheetcam? I only see overcut option, I mostly use the torch off rule to turn the torch off just as it gets to the lead out or very slightly before so although the machine keeps moving along the lead out the torch switched off before turning, works a treat at stopping that burnt blob on the hole edge.
I'm sure I tried not using a leadout and just having the torch off, I still got the burn mark doing that way though.
Cheers


In my software, I can program an overcut (the path continues on PAST where the lead in came into the cut path for the part, by a length that I specify, so I can either have a gap at the end of the loop, and come up short say 1/3rd of the kerf width, OR I can keep going and OVERCUT or cut back over the path, again by a length I specify) or I can have an overburn (simply leaves the torch ON at the end of the path, for an amount of time that I specify, so it will stay lit for x seconds after the end of the path is reached). It works GREAT for getting rid of that little tit you refer to especially when cutting smaller circles on thicker materials, such as 3/4 and thicker plate. On 3/4 and thicker I usually OVERCUT by 0.10" and also OVERBURN by 0.5 seconds, and the lead in taper is usually non existent. If I can tell where it was at all, it's only because I am the one running the machine and doing the cutting, the customer usually has no clue.

As far as lowering the cut height to true up the bottom of the circle, I have had better luck with this if I reduce speed by approx 30% as well, as this allows the arc to "hunt" for material if you will, and it will widen out or flare out at the bottom since it is attracted to the steel via arc transfer, and is looking for path of least resistance. I say that with my tongue in my cheek, as ASME specs say bolt holes should be 1/16" bigger then the nominal size of the fastener being used up to just under 1". At 1" it jumps to 3/32", and again at 2" it increases, so a 1/2" hole ( 0.5" ) should be 0.5625" in diameter, and I rarely get more than a 0.010-0.015" variance top to bottom on material that is 5/8" or thinner. On the thicker stuff, if it's a hole that is smaller than 1.5x the plate thickness, it's a PITA and I will usually just mark centers and use the mag drill and broach them, it's just as quick as chasing hole diameter all over the place, then using a double cut carbide burr to try and true them up (and getting those mother$#%&^@!!!@##@@! little sharp ass slivers all over EVERYTHING and in my hands, the crease of my elbow, creases of my fingers, ruining a pair of gloves, etc). Have I mentioned how crappy it is to use a carbide burr? It's the tool I love to hate. It can accomplish so much, yet make you hate it for days. The worst is when you think you have finally expunged all the little shits from the shop, and then grab a magnet or something and jab another one in your finger......

Another thing to note, which I am sure you know, is that as consumables wear your kerf increases, and angularity can change, and you can, in turn, pull all your hair out chasing hole diameters.


That last set of pics where you were cutting 1/4" look great, I know several people here in the states that wish they could run their machine good enough to cut parts like that. Several of them are my competitors. I even had one shop send a flunky out to make sure I was using plasma and not a waterjet, as a customer that used to be theirs, but was mine now took a piece in that I had cut to beat them up about their angularity. It was kind of funny, since the flunky came on his lunch break.... Wearing his uniform from the other place...... Complete with a patch with their name and all. I just grinned.


Be safe

Shane

[SeanP]

Thanks again Shane, I get it now, I'm going to have a try at that on some thicker parts, can do the overcut in sheetcam and I'm sure I will be able to make a rule up to overburn a little after the cut finishes.

I'm probably not making it easy for myself trying to cut to smaller holes really, but then I'm getting the tag holding the part into the sheet quite a lot on decent size parts, only on 8mm+ though.

I know just what you mean about about those slivers, I've only just started using those cutters, handy enough tool but nasty bits like you say
Cheers

Thanks Shane,
Some good points there, I'm not to far away to your recommendations, I don't quite follow the overburn part though, are you using sheetcam? I only see overcut option, I mostly use the torch off rule to turn the torch off just as it gets to the lead out or very slightly before so although the machine keeps moving along the lead out the torch switched off before turning, works a treat at stopping that burnt blob on the hole edge.
I'm sure I tried not using a leadout and just having the torch off, I still got the burn mark doing that way though.
Cheers


In my software, I can program an overcut (the path continues on PAST where the lead in came into the cut path for the part, by a length that I specify, so I can either have a gap at the end of the loop, and come up short say 1/3rd of the kerf width, OR I can keep going and OVERCUT or cut back over the path, again by a length I specify) or I can have an overburn (simply leaves the torch ON at the end of the path, for an amount of time that I specify, so it will stay lit for x seconds after the end of the path is reached). It works GREAT for getting rid of that little tit you refer to especially when cutting smaller circles on thicker materials, such as 3/4 and thicker plate. On 3/4 and thicker I usually OVERCUT by 0.10" and also OVERBURN by 0.5 seconds, and the lead in taper is usually non existent. If I can tell where it was at all, it's only because I am the one running the machine and doing the cutting, the customer usually has no clue.

As far as lowering the cut height to true up the bottom of the circle, I have had better luck with this if I reduce speed by approx 30% as well, as this allows the arc to "hunt" for material if you will, and it will widen out or flare out at the bottom since it is attracted to the steel via arc transfer, and is looking for path of least resistance. I say that with my tongue in my cheek, as ASME specs say bolt holes should be 1/16" bigger then the nominal size of the fastener being used up to just under 1". At 1" it jumps to 3/32", and again at 2" it increases, so a 1/2" hole ( 0.5" ) should be 0.5625" in diameter, and I rarely get more than a 0.010-0.015" variance top to bottom on material that is 5/8" or thinner. On the thicker stuff, if it's a hole that is smaller than 1.5x the plate thickness, it's a PITA and I will usually just mark centers and use the mag drill and broach them, it's just as quick as chasing hole diameter all over the place, then using a double cut carbide burr to try and true them up (and getting those mother$#%&^@!!!@##@@! little sharp ass slivers all over EVERYTHING and in my hands, the crease of my elbow, creases of my fingers, ruining a pair of gloves, etc). Have I mentioned how crappy it is to use a carbide burr? It's the tool I love to hate. It can accomplish so much, yet make you hate it for days. The worst is when you think you have finally expunged all the little shits from the shop, and then grab a magnet or something and jab another one in your finger......

Another thing to note, which I am sure you know, is that as consumables wear your kerf increases, and angularity can change, and you can, in turn, pull all your hair out chasing hole diameters.


That last set of pics where you were cutting 1/4" look great, I know several people here in the states that wish they could run their machine good enough to cut parts like that. Several of them are my competitors. I even had one shop send a flunky out to make sure I was using plasma and not a waterjet, as a customer that used to be theirs, but was mine now took a piece in that I had cut to beat them up about their angularity. It was kind of funny, since the flunky came on his lunch break.... Wearing his uniform from the other place...... Complete with a patch with their name and all. I just grinned.


Be safe

Shane