Overcut issue or ????

[Simko]

I just started cutting on my table a few weeks ago and all of that has been misc files out of 12ga.

A friend needed a few 1/2" gussets cut and had the plate so I jumped at the chance to cut something a little thicker than 12ga.

I did a few dry runs to make sure that pierce heights and cut heights were all book specs. Everything looked great so I decided to go for it.

The parts pierced and cut perfectly, but I am getting a nub at the end of my cut. I checked SheetCAM and the overcut was set to zero. Is this the variable that I need to adjust to get rid of the nub or is there something else I should be checking out?

3" x 3" gussets and slug from a 1" diameter hole

[SeanP]

Nice square cuts! you don't look to have much of a leadin on the round slug, might not help with that tab but would maybe get a better hole.
I can only get parts of 10mm up to drop out by having a slowdown rule, ie: say 4mm from end slow to 50% (not including leadout unchecked) and then say 1mm from end back to 100% you will need to experiment a bit with distance and slowdown rate, it just slows enough to catch that tag, it seem as if the arc skips as it passes from one side of the leadin to the other.
Maybe there are other ways as well but it definitely works for me.
I would have thought the 85 should have had less trouble from that than the 45 really though.

[plain ol Bill]

I use an overcut of .200 on 1/2" and have clean cuts. I would have a .250 lead in at least and maybe a bump more if your starts are showing.

[Simko]

Thanks for the responses!

So it seems there are at least two ways to skin this cat. Slow down or overcut. I will try both out and see which ones gives a better cut.

I don't know why I didn't think to make the lead-in bigger. I had it set pretty tight for the 12ga cuts to get the lead-in to fit in tight spaces and forgot to change it.

[Old Iron]

If mine would cut 1/2" that good, I'd be doing the cabbage patch dance around the table

[djreiswig]

Simko:
I've almost forgot to change my lead-in lengths in SheetCAM many times. I mentioned to Les that I thought it would make more sense to keep the lead-in settings with the tools since they are usually related to the material thickness being cut. The type is already there, but why not the style and length? Maybe if more people let him know their thoughts on this, it would move up on the project list.

Do you find you have any excessive beveling on the 1/2"? I sometimes run into trouble with mine looking like a parallelogram. Everything seems square and consumables look good. Sometimes it will cut great. Also, I sometimes have trouble with the tab on the end. I've played with overcuts and slowdowns limited success. Report back on your results.

[Simko]

If mine would cut 1/2" that good, I'd be doing the cabbage patch dance around the table

Simko:
I've almost forgot to change my lead-in lengths in SheetCAM many times. I mentioned to Les that I thought it would make more sense to keep the lead-in settings with the tools since they are usually related to the material thickness being cut.

Do you find you have any excessive beveling on the 1/2"? I sometimes run into trouble with mine looking like a parallelogram.

It does seem to make sense to have the lead-in settings save with the tool. But maybe there is something we're missing as to why Les left them out?!?

The beveling wasn't bad at all. I didn't get a lot of time to study the piece though. We were kind of in a time crunch. I looked at it quickly and took a few pictures. The hypotenuse had a little more beveling than the legs of the triangle for some reason.

Being my first 1/2" cut, I was just stoked to see it pierce and make the full cut without a lot of hassle.

[djreiswig]

Les said he had others mention the lead-in thing. Last I heard he was pondering it.

If you want to see something cool, try some 3/4". Or you could probably pierce 1" with your 85. I use a ramp pierce on the thicker stuff. No pierce delay and set the plunge the same as the cut speed to get a 45 degree ramp. Shoots a pretty impressive rooster tail.

[SeanP]

I must admit I do spend quite a bit of time adjusting leadin length and type, I'm not sure about saving with tools would be better or not really, one thing that is a good time saver is on the development version is a option to start at centre of holes under a preset size.

I've never had much joy with the overcut feature to be honest.

[jimcolt]

The lag lines indicate that your cut speed might be too fast....though it could also be height slightly too high. 1/2" cuts at the right speed and height should drop, even if done at 45 Amps. Overall they look good. Thicker is generally easier to dial in cut quality than gauge material.

For DJReiswig: When you get severe beveling in a parallelogram fashion....you have a damaged nozzle. Look carefully at the nozzle and shield orifices with a 10x eye loupe, you will see a notch or crater that affects the shape of the arc. Damage to the nozzle is most commonly caused by incorrect pierce height and pierce delay time.

Jim Colt Hypertherm

I just started cutting on my table a few weeks ago and all of that has been misc files out of 12ga.

A friend needed a few 1/2" gussets cut and had the plate so I jumped at the chance to cut something a little thicker than 12ga.

I did a few dry runs to make sure that pierce heights and cut heights were all book specs. Everything looked great so I decided to go for it.

The parts pierced and cut perfectly, but I am getting a nub at the end of my cut. I checked SheetCAM and the overcut was set to zero. Is this the variable that I need to adjust to get rid of the nub or is there something else I should be checking out?

3" x 3" gussets and slug from a 1" diameter hole

IMG_4314.JPG

IMG_4315.JPG

[djreiswig]

I've had it happen with a new nozzle.

[Simko]

The lag lines indicate that your cut speed might be too fast....though it could also be height slightly too high. 1/2" cuts at the right speed and height should drop, even if done at 45 Amps. Overall they look good. Thicker is generally easier to dial in cut quality than gauge material.

I ended up using an 85A tip because I did not have any 65A. Could that have something to do with it? I verified 85A book specs (pierce/cut height/speed), but to tell you the truth, I didn't look at the volts it was cutting at because I was watching the cut.

The CandCNC manual says to make a few straight cuts on flat material at the cut height with the THC off and use that voltage for the material instead of the book voltage. Is it worth changing if its 2-3 volts different from the Hypertherm book spec? I figured it was slightly off due to the material not being perfectly flat or my slats not being perfect.

[steel 35]

If you test it and get a number 1 or two off cut at those numbers instead of book, didn't read where you are cutting at 60% holes rule? and I use .125 overcut and .1 arc lead out, works good for me. I run into trouble using other slow down rules.

[SeanP]

If I was cutting those I would turn off thc (with the creen button) for that size, or if you wanted to set it on the next part just see what the torch volts cuts at and then match it on the preset volts. certainly turn off for holes under 30mm you don't want it on, best to set up cut rule for holes as you want to be 60% feed rate reduction.

[Simko]

certainly turn off for holes under 30mm you don't want it on, best to set up cut rule for holes as you want to be 60% feed rate reduction.

Is this true even with the velocity anti-dive feature of CommandCNC where it will turn off the THC automatically if the speed drops below a certain percentage of cut speed (right now at 85%).

There are a lot of tweaks and tricks that I have yet to learn to make consistent good cuts.

[SeanP]

Ah sorry, I'm not sure about that, I'm getting left behind on the older version!

[tcaudle]

In SheetCAM with a current POST you have a setting in the Operations called "Min Cut Length for DTHC" If you set that length to a value Greater than the total cut length (circumference + lead in) then the DTHC never turns on. Commandcnc tracks the toolpath and adjusts the velocity to keep the cut inside the abilities of the mechanics rather than alter the toolpath to get max speed. As a result the VAD works much better because the motion is constatnly being changed and it detects that instantly. If you lower the feedrate in SheetCAM then it may be able to cut at the full speed you assign and VAD will not cut in. For those circumstances on smaller cuts (holes or other shapes) you have the Min Cut Length fo DTHC setting. Its a much better way to control the DTHC than using Cut Rules because its already off at the beginning of each cut and it can look ahead and determine if it needs to turn on. If you put the DTHC OFF cut rule in the wrong place, it will not keep it from turning on automatically

[Simko]

Thanks Tom. That helps a lot!

[Brand X]

I would not use 85 amps for best quality on .500 simple as that.. Depending on shape, the loop corners (Triangle) Tangent lead-in, and out can get excellent results.. Don't make me post my Thermal dynamics .750 ms cut at 60 amps.. So I will post a 90 amp cuts out of 1 inch MS (Esab)
one inch cube..

[Simko]

I would not use 85 amps for best quality on .500 simple as that.. Depending on shape, the loop corners (Triangle) Tangent lead-in, and out can get excellent results.. Don't make me post my Thermal dynamics .750 ms cut at 60 amps.. So I will post a 90 amp cuts out of 1 inch MS (Esab)
one inch cube..

Nice cuts! ... I agree, but all I had was 45A and 85A nozzles. The PM 65/85 book doesn't have settings for 1/2" at 45A, so I went with 85A. I do recall reading somewhere that the new 45XP will cut 1/2" and you can use the same settings on 65/85/125. I have seen some tool sets around that incorporate these new numbers, but I haven't downloaded one yet.

[Brand X]

45 would work.. Standard model 45 specs was used before the 45 XP came out.. I've seen my friend cut with 65 amp book specs, and it was just excellent. Tons of brackets, and i looked them all over good.. Was really better then I could get with my Hypertherm 65. I could really do better with my Victor or Esab. Comes down to the person running the machine, more then the machine.. (IMO) Lot of times it gets totally blown out over brand, and it's just not so as far as cut quality cut goes..With me there was things I liked about the 45, and 65 amp cuts, and things I did not like.. Pick what you think is important, and go with it.. Just the little things matter, and add up to great cuts.. Friend cut his with the THC off too.. I sure he referenced each cut was only about 6-8 inches in size overall . Pretty complex shape,so you could see he had it dialed in 30 ipm book 65 amps.. Quality of steel is huge too.. He gets good stuff..