holes and bevel

[waynehartwig]

I was cutting some holes in 1/4" plate yesterday (.34" for a 5/16 bolt) and part of the hole had a large bevel, where part of it was straight.

Explained better: it pierces and runs counter clockwise (IIRC) to about 1/3 of the hole and there is no bevel. For the last 2/3's of the hole there is a significant bevel. To the point the 5/16 bolt will not fit through.

Any thoughts?

A120 machine set at 60A/consumables and 55 IPM.

I found that my table is unsquare (off 1/4" from front to back) to the head and since I'm trying to lower the table 1" (increase the distance from 4-5" under the head), I'm cutting new slat supports and mounts and fixing the square issue at the same time.

[SoundManCO]

I have been marking the holes with the 2x2, just a small pierce, then take them to the drill press for a much cleaner hole that needs 0 cleanup after.

[BESRK]

Usually, if I find my holes starting to taper on one side only, it's because the nozzle is worn. However, that's irregardless of cutting a hole, straight line..etc.

Maybe the arc feedrate is kind of high? For the first part of the hole, the torch speed could be ramping up... since it's a bit slower, it might cut okay for a bit then begin to taper as it gets up to speed? Just a thought..

[HardcorewannabeXJ]

60 amps at 55 i/pm is not going to give you a good small hole in .25" material. For the best (roundest) holes, they recommend running the small holes at 60% of the straight line program feedrate. The slower the cut is the torch has more time to consume material and catch up to keep the flame straight. Or you can cut the .25" material at 80 amps and you'll probably get a cleaner small circle cut.

To set the arc motions at a certain speed, go to the Configuration - Machine - Feedrate Ramping panel. On this screen, there is a Maximum Arc Feedrate, set this to 60% of your program feedrate and you should see better holes. Keep in mind this will limit all arc motions, even larger radiuses that may not need to slow down.

[waynehartwig]

Problem is I do a lot of holes, so marking/drilling isn't really a viable option.

The tip is new. I pulled it and it still looks new. The hole is still nice and round. So I don't think it's the tip this time.

I'm not sure I want to run 80A on 1/4", so I'll try slowing down the circls first.

What do the Fd Rate linear and rotary do?
They are set at:
ARC FeedRate - 100 in (just lowered it to 25 ipm per your recommendation)
linear is - 50 in
rotary is - 720 in

The biggest hole I will be cutting on my table is probably 15/16", for clevis pins. But mostly they are 1/4-5/8". The bigger ones for the recievre tube and clevis pins don't matter, because I'll be welding them up afterwards. The other holes are also in .120-.188 material as well.

Thanks!!!!!!

[BESRK]

I don't have my notes here with me but for pretty clean cuts on 1/4" (with my Hypertherm 1250 and 40amp nozzles), I cut it at 40amps and around 45ish ipm straight line and about 30ipm in the arc... give or take a couple ipm.

I oversize bolt holes about .020" and am able to get a bolt thru it. That's for typical 5/16"-1/2" bolts or so..

[waynehartwig]

Originally Posted by BESRK

I don't have my notes here with me but for pretty clean cuts on 1/4" (with my Hypertherm 1250 and 40amp nozzles), I cut it at 40amps and around 45ish ipm straight line and about 30ipm in the arc... give or take a couple ipm.

I oversize bolt holes about .020" and am able to get a bolt thru it. That's for typical 5/16"-1/2" bolts or so..

Thanks!

[Conrad_Turbo]

Originally Posted by HardcorewannabeXJ

To set the arc motions at a certain speed, go to the Configuration - Machine - Feedrate Ramping panel. On this screen, there is a Maximum Arc Feedrate, set this to 60% of your program feedrate and you should see better holes. Keep in mind this will limit all arc motions, even larger radiuses that may not need to slow down.

Just digging this back up as I have been cutting some 3/16" MS with a 65A nozzle @ 65A with my PM65. I am cutting some small 1"x1.5" tabs with one 0.344" diameter hole @ 140IPM, 0.15 pierce height and 0.06 initial cut height and running AVHC. I don't have any 45A nozzles (they're on order right now) so for right now I'm assuming I can improve the hole quality by slowing things down, however when trying to change the Maximum Arc Feedrate setting, it is grayed out and listed at 100in/min. I am using Version 4.0.45 of the TM controller software.

[HardcorewannabeXJ]

Originally Posted by Conrad_Turbo

Just digging this back up as I have been cutting some 3/16" MS with a 65A nozzle @ 65A with my PM65. I am cutting some small 1"x1.5" tabs with one 0.344" diameter hole @ 140IPM, 0.15 pierce height and 0.06 initial cut height and running AVHC. I don't have any 45A nozzles (they're on order right now) so for right now I'm assuming I can improve the hole quality by slowing things down, however when trying to change the Maximum Arc Feedrate setting, it is grayed out and listed at 100in/min. I am using Version 4.0.45 of the TM controller software.

You will have to take the software out of the "express mode" which can be done when disconnected from the control box by going to the Configuration - System - Controller menu. The next time you connect it will adjust the firmware on the main board of the control box, and you will be able to adjust the max arc feedrate then.

-Mike

[Conrad_Turbo]

Awesome thanks Mike! Now with it listing a Max Arc Feedrate, do I have to change this every time I am cutting a different thickness material? Or is there a way to have it work as a % of the cutting feedrate? In other words setting it up to 60% of whatever the feedrate may be for the material being cut?

[DLE]

Man im glad someone else just asked this question. I've been baffled why I couldn't adhjust the MAF.

[BESRK]

Originally Posted by Conrad_Turbo

Awesome thanks Mike! Now with it listing a Max Arc Feedrate, do I have to change this every time I am cutting a different thickness material? Or is there a way to have it work as a % of the cutting feedrate? In other words setting it up to 60% of whatever the feedrate may be for the material being cut?

Once you get everything dialed in for a particular material/thickness/amperage/nozzle type, save the setup as its own file.. for example "3/16" Steel with 40amp Shielded Nozzle".. or "1/8" Steel with Fine Cut Nozzle"....etc.

Then, when you change out material/thickness/nozzles, you can just open the setup file for that combination and the driver program is already dialed in.