Hey everyone! I have a Hypertherm Powermax 45XP on my CrossFire Pro table that I’ve been using for a while and its been working great. I recently moved and was resetting it up and figured I’d try to get this question answered because I think I must be doing something really dumb.
The problem I’m having is that I have to make pretty much all cuts much slower then the Powermax 45XP cut sheet implies. For example, today I tried cutting some 12 gauge – which according to the cut settings sheet should be cut at over 100ipm at 45amp. In my case (using SmartVoltage) this would not pierce the material fully until I backed it down to about 60ipm, at around 50ipm I got (what I think) is a perfect cut (low dross, nice flat sides, etc). In the past I was more or less content with just cutting slow, but I feel like I might just be doing something wrong as other folks seem to be able to cut at much higher ipm.
If you take some time to read other posts you will see that most things eventually need to be discovered by you systematically ruling out possible causes. That being said I want to get a bit more detail from you.
The more information that you can supply, the better we can try to help. We need this:
(note, this is a form text so you may have already supplied some of the following or may not be necessary right now. If that is the case, I will try to strike-through). • Do a sample design, something simple like a 2 inch x 2 inch box with a 3/4 inch circle in the middle of the box. Manufacture the gcode and attempt to run it on your setup. Report your results and share the gcode.
• CAD program used
• CAM program used (SheetCAM or Fusion 360)
• metal thickness/type…you said 12 gauge so I assume you mean mild steel???
• work lead attached to shiny/clean metal
• work lead, torch cable, THC cable and printer cable to the enclosure are not touching/crossing paths nor coiled up
• copy of the gcode of your test file
• photo of how your torch is mounted
• photos of your consumables
• photo of your VIM box so we can see what leads and connections are used
• Are you using OEM consumables? Are they standard or fine-cut consumables.
• What is the brand of the consumables (not the machine they are labeled for)
• air quality and quantity (pressure gauge at the plasma cutter), what methods of drying employed. You need 6 CFM @ 90 psi and it needs to be dry.
• Do you have the THC? If so, are you using “Smart Voltage” on “nominal voltage”
• Have you had any successful cuts with the current setup and metal type/thickness?
• Is there any connection issues with the IHS contacts in the z-axis carriage?
• Have you lubricated the lead screws?
• Are you using a laptop and is it plugged in or running on battery only? Fully charged?
• Cut height: have you measured what your cut height actually is when you set it at 0.06 inches for normal consumables and 0.14 for Hypertherm SYNC consumables?
Note: You will be able to supply attached files such as photos after you have posted a few more times. For videos, upload to a service like YouTube and then provide a link to your video. For gcode file you can open it in a text editor and copy the text and paste in a post. If you are needing to post the gcode by copying the text, just copy the first 20 lines for now.
Thank you! I was using .4 pierce delay, let me try .6 and see how that goes. Will report back!
As for details from ChelanJim, here is what I got –
• CAD program used – Fusion 360
• CAM program used (SheetCAM or Fusion 360) – Fusion 360
• metal thickness/type…you said 12 gauge so I assume you mean mild steel??? – That’s right, sorry, just normal mild steel.
• work lead attached to shiny/clean metal – It’s attached to the part being cut, but its got some mill scale on it for sure, let me clean it.
• work lead, torch cable, THC cable and printer cable to the enclosure are not touching/crossing paths nor coiled up – This is the case yep, I just re set up the machine and things seem to be properly set up here. Let me double check the point about the THC cable.
• copy of the gcode of your test file – Pasted below (it says new users can’t upload attachments).
• photo of how your torch is mounted – Will attach once I can. I’m using the hand torch, not machine torch.
• photos of your consumables – Will attach once I can. I just recently replaced them with new, maybe less then 5 cuts on these new ones.
• photo of your VIM box so we can see what leads and connections are used – Will attach, but I am using RAW voltage input and the PV output.
• Are you using OEM consumables? Are they standard or fine-cut consumables. – These are OEM from Hypertherm, standard and NOT fine-cut.
• What is the brand of the consumables (not the machine they are labeled for) – they were marked Hypertherm on the box.
• air quality and quantity (pressure gauge at the plasma cutter), what methods of drying employed. You need 6 CFM @ 90 psi and it needs to be dry. – I’m at about 100-110 at the regulator with a short (4-5 ft) hose to the machine. I’m using an aftercooler for the compressor and a refrigerated air dryer before the plasma cutter. Compressor is 80 gallon, 16 scfm (advertised), 3/4 lines.
• Do you have the THC? If so, are you using “Smart Voltage” on “nominal voltage” – I’m using Smart Voltage for the cuts in question.
• Have you had any successful cuts with the current setup and metal type/thickness? – Yes! If i slow down to ~60 ipm I get great quality cuts.
• Is there any connection issues with the IHS contacts in the z-axis carriage? – Nope, at slower speed everything works great.
• Have you lubricated the lead screws? – I have not, but I should probably do that!
• Are you using a laptop and is it plugged in or running on battery only? Fully charged? – Laptop is fully charged and plugged into the wall.
• Cut height: have you measured what your cut height actually is when you set it at 0.06 inches for normal consumables and 0.14 for Hypertherm SYNC consumables? – I have not, I’ve just been using the default 0.063 height.
Here is the gcode (this is me experimenting at 200ipm, I then used the Langmuir software to tune it all the way down to 30% to produce 60ipm where I got good cuts, I tried 100ipm along the way down too):
The main thing is that I can get awesome cuts if I slow down to ~60 ipm, that’s what I’ve been doing up to this point – since I’m not running a production environment going slower is really no problem, I just wanted to figure out why I’m getting this behavior.
I am very impressed with your response. Thank you for taking the time to do that.
As David implied, pierce delay could make a big difference. If you don’t get the metal pierced adequately, it will continue to compromise the torch’s ability to cut.
The next thing is the cut height. If the height is too high, it is going to take longer to pierce the metal and adequately clear the kerf path. Theory: Perhaps your cut height is off and is too high. Slowing the torch gives extra time to clear the metal out of the kerf.
Normally when then cut height is too high you will get more dross on the top of the plate you are cutting and you will get a bevel (positive) that encroaches the kerf path. You may not get the bevel because you have slowed the speed of the cut.
If the cut is too slow you will get a significant undermining bevel of the plate (considering that the cut height is set correctly).
Another thing is that your nozzle could be worn excessively. In this case I could see a scenario where you had a normal cut height or too low of a cut height but due to the inefficiency of the cut due to the widening spread of the plasma stream, you are not getting adequate clearing of metal. Your cut speed being slower is giving a chances to complete the cut but I would expect this to have a significant negative bevel (undermining the plate).
Looking forward to seeing some photos. Try David’s increased pierce delay. Measure your actual cut height and get back to us.
I see the line with the springback and backlash has a value of .040". That probably means that you are cutting at .100" instead of the .063" that you programmed.
Both of those compensations are mostly unnecessary and add unwanted pierce and cut height. You can eliminate the springback portion by setting it to zero, but the backlash is baked into the post processor. I don’t use Fusion, so i just reduce my cut height to eliminate it. You may be able to set a negative value in the Springback field in Fusion.
Wow! OK so I got it to cut great at 100ipm. I changed the springback to -.02 which corrected the height to .063 as intended. I also changed the pierce delay to .06. At first it wasn’t quite cutting consistently, but after playing with it for a bit I realized what I did wrong.
Some time ago someone suggested in a different thread to use a soft silicone funnel upside down around the nozzle to contain the sparks and splashes. I realized that in some cases this funnel was obstructing the IHS when it was initially measuring the distance to the plate (it would cause it to trigger sooner then when the torch hit the plate). I think this in turn caused the Smart Voltage to run at a lower voltage then required and caused my issues (I was basically trying to cut at a much lower voltage then what I should be using!).
I removed the silicone funnel and the cut went perfect at 100ipm with the settings suggested above. I’ll have to think up a better anti-spark/splash method to ensure it doesn’t obstruct the IHS.
Thank you so much for all the feedback and information! I will keep these settings locked in for all my future cuts!
Excellent. Yes, a photo would have helped but you did a great job following David’s advice and helped track it down.
I saw those funnels used by others and it just seemed “too much going on” around the torch nozzle for me. Plus, it interferes with your ability to change the consumables (depending on your setup). Everyone has their own setups and needs.
I use one every day. It’s great not to have the sparks and arc that blind me. It pulls right off to change the consumables. Just my two cents.
It has never affected my cuts or IHS.
How do you have this set up? I have a few in my toolbox that I was contemplating adding (not till i get my other issues sorted out). What did you use to cut out the torch provision? I’ve been using some angle iron around the table edges, but the crash likelihood worries me about continuing to do so.
I think in my case perhaps the funnel was not soft enough? I did notice it get jammed up sometimes against the material being cut when I was moving the torch around manually and it happened to be too low. I think in my case I was chasing multiple issues – the pierce delay, height being too high, and the funnel was creating intermittent issues with the height being inconsistent affecting the voltage (when using SmartVoltage – which I use). Basically I had a whole host of issues going on! So for some the funnel might work just fine!
