Problem cutting 3/4", Jim Colt and others opinion please....

[Charlieboy]

I am running a hypertherm powermax 105 on a Torchmate X table. The hypertherm is 3 phase and runs off of a phase converter (if that matters). I was running an 85 am consumable at 21 in/min. Brand new consumables. I cut 21 of these plates total. 1' x 1' with 3/4" inch size holes. I went through and pierced all of the holes first and them went back to complete the cuts. From the top side the cuts looked great, but when I started pulling parts off table, that was not the case.
I really need some help on this. The machine will cut 3/16" all day long, but the thicker plate is giving me hell.

[cbassjr]

Ran into exactly the same problem when I stepped up to 1/2" on a recent production run. Are you running THC, Sheetcam and Mach 3? If so I may be able to help. In Sheetcam under Options - Job Options you need to set your Plunge Safety Clearance to 1.2 and make sure your setting are correct match to your Hypertherm manual setting match material and consumables. In Mach 3 when you type in your proper temp from the manual you need to then click on the THC button with the up and down arrows to the left of where you entered your temp. As you are cutting you can adjust the THC with the up and down arrows to dial in your THC. The key here is clicking on that THC icon as even though you entered the temp it is really cutting at the Mach 3 default temp. Made all the difference in the world for me Holes were perfect and cuts were perfect. Hope this helps.

[Charlieboy]

I appreciate your reply, yes I am running THC, and I am running the software that torchmate provides. I am not familiar with sheetcam, but I am cutting in the torchmate driver software. Is that similiar to sheetcam or the other software that you mentioned?

[Charlieboy]

This is the reply that tech support gave me, let me know your opinions please.


The few things that I notice right off the bat are that the holes seem to be a little small for what we recommend when it comes to the thickness of material you are cutting. We recommend a 2:1 ratio where the diameter of the hole is at least 2 times the thickness of material. It also looks as though you are not piercing long enough. Try increasing the pierce delay a little bit more so that you get a full complete pierce before the machine starts to travel. I also noticed that the picture of the one cam follower that is loose. It may cause some binding if it gets twisted the right way. Hope this helps.

[icmplasma85]

I will agree with what tech support says to a certain point. I don't think you need quite a 2:1 ratio, but it certainly is difficult to cut a hole the same diameter as the thickness of the plate. On 3/4" thick plate, 1" diameter holes are probably the smallest that you can get to look acceptable. It's like trying to cut a 1/4" hole in 1/4" plate, you will have a lot of taper in the hole. Best to mark the hole locations and drill after the part is cut instead of plasma cutting the holes. Don't know if you can do this with your software, but certain programs will allow you to mark the center of the holes with a point function. You set the time to mark point at a much lower number that your pierce delay so that the torch makes a quick "blip" right where the center of the hole should be. If I am cutting, say, 1/4" plate, I will only plasma cut 3/8" or 1/2" holes, with the latter looking much better than the 3/8". If you can mark hole centers with your software that would be the best route for this project.

If you must cut the holes, and the customer has some room for error, try cutting a 13/16" or 7/8" hole even though you need a 3/4" hole. After the taper on the bottom of the plate, you will probably be close to the dimension you need. Hope this helps.

[jimcolt]

From the looks of your holes there are a few things you can do for improvement:

1. Speed for all holes under about 1-1/4" diameter should be programmed at 60% of the best quality "book" speed. The book speed for 3/4" steel using the 85 amp shielded consumables is 24 ipm.....so cut your holes at about 15 ipm. This will improve taper, and will help with the end of cut lag in the arc that does not allow the slug to drop. Expect low speed dross on the bottom, however it will knock off easily.

2. Physical cut height is extremely critical for holes. Ensure that the torch is settling to the correct cut height before the x and y motion gets on the hole radius. Your lead in needs to be long enough so that the torch indexes from pierce height to cut height before leaving the lead in. Absolutely critical.

3. If you software cannot automatically keep the arc voltage feedback height control from functioning (on all holes under 1.25" diameter)....then put the height control in manual for all of these holes. Because of the slower speeds...the arc voltage height control will not work well...and will cause the bottom of the hole to be out of round.

4. Program the end of the hole with an overburn if your software allows it.This means to stay on the hole radius (do not lead back into the center) for about .150" past the lead in kerf. This will help "finish" the cut with a smoother transition.

5. You may get better results using the 105 amps shielded process with the above techniques on 3/4" plate.

6. Expect about .030" to .045" taper in these holes. Bottom will be smaller than the top. Adjust hole size to accommodate this.

Jim Colt Hypertherm

[Charlieboy]

I appreciate both of the replies, this puts more confidence back into my machine. Do you think that there is a moisture problem in the air supply. The shop has a couple hundred feet of airlines running through the building, but I only have an air/water separator on the line. I have spoke with my local supply company about a nitrogen pack to test and see if that will improve the cuts. Or should I just invest in a refrigerated dryer?

[Shane Warnick]

Get a refrigerated dryer and don't look back. If you are asking, yes there is moisture. There always is. Even with a refrigerated dryer I am still changing desiccant once a week or so. I can tell you my consumables last a lot longer and mu cut quality is way better.

As far as the holes, I echo what Jim says. Manual THC, (let it just cut at a height you shouldn't be seeing the material move at all on a hole like that in plate that size anyways) . I also agree on the over burn. On my machine I can set the gap at end of loop to a negative number, and cut past the lead in into the arc of the circle again and finish out the bottom of the hole. I set up a second operation on plate thicker than 1/4" and have one set up for small holes, and then the other just for perimeter cutting etc. A 2:1 ratio seems high on thickness vs diameter to me though. I don't go below 1:1 and can cut holes with minimal taper with my Powermax 1250.

Shane

[jimcolt]

If there is moisture in your air lines you will find evidence of it in your water separator. It will not cause cut quality issues (on a Hypertherm) with a new set of consumables unless the issue is real severe....rather it will cause your consumables to wear faster than they should....so you will see deterioration in cut quality over time....I don't see that in your pics.

Nitrogen will definitely make your cuts worse. Air has a 20% oxygen and 80% nitrogen content (roughly)...the oxygen content provides an exothermic reaction with steel with the result of squarer, cleaner edges and faster cut speeds. Nitrogen will be slower, worse angularity and more dross.

Jim Colt Hypertherm

I appreciate both of the replies, this puts more confidence back into my machine. Do you think that there is a moisture problem in the air supply. The shop has a couple hundred feet of airlines running through the building, but I only have an air/water separator on the line. I have spoke with my local supply company about a nitrogen pack to test and see if that will improve the cuts. Or should I just invest in a refrigerated dryer?