Problem- poor quality cuts in X-axis

[brogger00]

Hi Everyone,

I was wondering if you might be able to shed some light on an issue I am having at the moment:

I am not getting quality cuts in the negative x-axis on my table, the positive x-axis cuts look good, but negative does not cut through the metal it just brushes along the top until the torch changes axis/direction. I always see the tell-tale sign of a bad cut, sparks flying everywhere above metal, voltage spikes from 80 to 100-115, and I see the molten metal on top of the material.

I know this sounds ridiculous and sounds more than likely a consumables issue but I have changed them out several times and this continues to happen.

I am using a hypertherm 1650 with fine cut consumables and operate at 50 amps, 70 ipm and only cut 11ga stainless.

I looked at the motor tuning and setup all the axis again. Then looked at acceleration, made a couple test cuts and there was virtually no difference in any of them. I thought maybe there was some dirt/oils/added resistance on the material so I began wiping it with a clean cloth prior to cutting, no effect.

The material is not warping at all when I cut so the THC is not the issue.
The air is of fine quality, the compressor is brand new with a water separator. Water level in table is not too high. Grounding also should not be an issue, I clamped right to metal and still no differences.

The last thing I continue to see is nozzles tend to be completely blown out after a mere 50 or so cuts, which is a direct result of the poor cuts being made. I cut out about 10 copies of everything I make and I see absolutely zero consistency between my cuts. One will be perfect, another will have a slight bevel (about .1"), the next will not cut properly. The whole situation at the moment is mind-boggling and I have been racking my brain since Monday to come up with an answer.

Any help would be greatly appreciated.

Thanks,

Brendan

[hub]

I'm just guessing here...
One "direction" is using conventional and the other climb milling? Maybe change the programming?

[brogger00]

Originally Posted by hub I'm just guessing here... One "direction" is using conventional and the other climb milling? Maybe change the programming?

Hi Hub,

I do not think it is the programming as all I have really been trying to cut are squares and circles, very simple things.

What is climb milling? Also if this were the case, how would I be able to find a solution? I am using Mach3 as a controller.

Thanks,

Brendan

[EBC]

http://www.cnczone.com/forums/woodwo...l_cutting.html

[hub]

Originally Posted by brogger00 Hi Hub, I do not think it is the programming as all I have really been trying to cut are squares and circles, very simple things. What is climb milling? Also if this were the case, how would I be able to find a solution? I am using Mach3 as a controller. Thanks, Brendan

I read your post through again, and you said torch.. So I'm guessing it's a plasma?
Conventional/climb milling applies to mechanical milling only.

I don't have experience with plasma so I can't be of much help.
Maybe (very wild guess) use more current if possible to make sure it cuts through?
It doesn't make sense to me why it works in one direction and not in the other.

Hub

[jimcolt]

A few suggestions based on what you have written below. If it truly is cutting differently when travelling in opposite directions…then there has to be something that is going on different based on motion. The plasma cannot tell direction….therefore if a plasma problem….I would expect some random occurrences in any direction.

Things that can be directional: 1. Differences in velocity, an if using arc voltage based THC…a velocity change will naturally change the height. 2. Motion roughness…mechanical issues.3.Torch to plate squareness.

From your pictures…and your plasma settings…I will offer some advice.

1. Use the 220404 deflector shield with the Fine Cut consumables. It extends beyond the nozzle and offers some protection from double arcing…….which I can see is occurring in your nozzle orifice.
2. While the Hypertherm manual suggests 50 amp cutting with FineCut consumables…I do not suggest going over 40 amps. I was on the original design team for these consumables…and they were designed with a 40 amp maximum rating. At 50 amps…..and especially without the 220404 shield…..the nozzle orifice will get damaged on one contact with the plate…or with a single piece of plate slag that touches the nozzle while cutting.
3. A nozzle damaged from double arcing wears the outside of the orifice to an out of round shape. This, in theory could cause directional cut quality issues.


I would suggest you use the following for 11 ga SS:

Consumables:

Deflector….220404
Retaining Cap….120928 (if using ohmic contact (I don’t know what height control you have) use 220061)
Nozzle…220329
Electrode…120926
Swirl Ring…120925

Amperage 40
Pierce height: .15”
Pierce delay time: .6 seconds
Cut height: .010” (yes, very close….and you must use 220404 shield to do this)
Cut speed: 80 ipm (may try a little faster or slower….my guess is that this is close)
For cut height: Don’t worry about arc voltage…..adjust the arc voltage during steady state cutting to achieve .010” cut height. As the consumables wear….you may have to ad as many as 10 volts to maintain the height.


Hope this helps,

Jim Colt

Originally Posted by brogger00 Hi Everyone, I was wondering if you might be able to shed some light on an issue I am having at the moment: I am not getting quality cuts in the negative x-axis on my table, the positive x-axis cuts look good, but negative does not cut through the metal it just brushes along the top until the torch changes axis/direction. I always see the tell-tale sign of a bad cut, sparks flying everywhere above metal, voltage spikes from 80 to 100-115, and I see the molten metal on top of the material. I know this sounds ridiculous and sounds more than likely a consumables issue but I have changed them out several times and this continues to happen. I am using a hypertherm 1650 with fine cut consumables and operate at 50 amps, 70 ipm and only cut 11ga stainless. I looked at the motor tuning and setup all the axis again. Then looked at acceleration, made a couple test cuts and there was virtually no difference in any of them. I thought maybe there was some dirt/oils/added resistance on the material so I began wiping it with a clean cloth prior to cutting, no effect. The material is not warping at all when I cut so the THC is not the issue. The air is of fine quality, the compressor is brand new with a water separator. Water level in table is not too high. Grounding also should not be an issue, I clamped right to metal and still no differences. The last thing I continue to see is nozzles tend to be completely blown out after a mere 50 or so cuts, which is a direct result of the poor cuts being made. I cut out about 10 copies of everything I make and I see absolutely zero consistency between my cuts. One will be perfect, another will have a slight bevel (about .1"), the next will not cut properly. The whole situation at the moment is mind-boggling and I have been racking my brain since Monday to come up with an answer. Any help would be greatly appreciated. Thanks, Brendan

[brogger00]

Hi,

EBC:

Thanks for the info.

Hub:

Following your climbing mill post I immediately google searched and realized that it could not be the issue.

The issue with increasing the current is that it will wear down the consumables at a faster rate as I am already using them at the higher end of the work range. Secondly, and this is more of a work related issue, my boss (the machine I use is only at work) wants the slugs to be in perfect working order. This is basically impossible, but he wants cuts that are 120% perfect, so increasing the amperage would damage the quality of the slug.

At this point in time the situation has changed drastically. For some reason the torch is now misfiring and welding the nozzle orifice close, therefore inhibiting me from even cutting at this point.

I really appreciate the help.

Brendan

[brogger00]

Originally Posted by jimcolt A few suggestions based on what you have written below. If it truly is cutting differently when travelling in opposite directions…then there has to be something that is going on different based on motion. The plasma cannot tell direction….therefore if a plasma problem….I would expect some random occurrences in any direction. Things that can be directional: 1. Differences in velocity, an if using arc voltage based THC…a velocity change will naturally change the height. 2. Motion roughness…mechanical issues.3.Torch to plate squareness. From your pictures…and your plasma settings…I will offer some advice. 1. Use the 220404 deflector shield with the Fine Cut consumables. It extends beyond the nozzle and offers some protection from double arcing…….which I can see is occurring in your nozzle orifice. 2. While the Hypertherm manual suggests 50 amp cutting with FineCut consumables…I do not suggest going over 40 amps. I was on the original design team for these consumables…and they were designed with a 40 amp maximum rating. At 50 amps…..and especially without the 220404 shield…..the nozzle orifice will get damaged on one contact with the plate…or with a single piece of plate slag that touches the nozzle while cutting. 3. A nozzle damaged from double arcing wears the outside of the orifice to an out of round shape. This, in theory could cause directional cut quality issues. I would suggest you use the following for 11 ga SS: Consumables: Deflector….220404 Retaining Cap….120928 (if using ohmic contact (I don’t know what height control you have) use 220061) Nozzle…220329 Electrode…120926 Swirl Ring…120925 Amperage 40 Pierce height: .15” Pierce delay time: .6 seconds Cut height: .010” (yes, very close….and you must use 220404 shield to do this) Cut speed: 80 ipm (may try a little faster or slower….my guess is that this is close) For cut height: Don’t worry about arc voltage…..adjust the arc voltage during steady state cutting to achieve .010” cut height. As the consumables wear….you may have to ad as many as 10 volts to maintain the height. Hope this helps, Jim Colt

Hi Jim,

I will certainly look into this.

Thank you very much.

Brendan

[brogger00]

Hi,

Thanks for the input everyone, now everything is running extremely well.

It looks like the issue turned out to be a combination of pierce height, pierce delay and cut speed.

Over the past several days I was able to make over 300 cuts using one nozzle and having them all come out at top quality.

Thanks,

Brendan