Help with CNC router set up/parameters/etc

[FickFab]

Hey everyone, hopefully this is the right section to post this, and thanks in advance for anyone that takes the time to read this and offer their input and knowledge/experience. We picked up a 4' x 8' Precix CNC Router early this year, ended up needing a TON of work but we have the machine up and running as of a few months ago and now we are just trying to get everything dialed in and set up and that is where we are looking for some help from someone that has experience with the below. I may not say things correctly, the terminology etc is all still relatively new to me so please excuse any confusing terms I might use incorrectly lol!

So the machine is an early model Precix CNC Router, it has a 48 x 96 cutting area, Perske 3hp 3 phase motor running off a VFD for our single phase power with a Max RPM of 18,000. The machine has servo motors and has only a single motor drive for the X axis to move the gantry, and a phenolic top. We have a MDF spoil board and are using a misting nozzle with Kool Mist 78 and then we have a second nozzle that is just compressed air, we run about 75PSI to the two nozzles so lets say 37PSI each. We are using the machine to cut 1/8" sheets of 5052 aluminum and this is where we are running into some problems, we are having to "babysit" the machine while it is running as it keeps welding the endmill and we just aren't sure what we need to change or do differently to be able to confidently leave the machine to run the program while we work on another project. We originally were using 1/8" 3 flute carbide endmills and were running the machine at 18,000 RPM and found that 20 IPM seems to be about as fast as we can go or the problems get worse. We secure the sheet to the MDF using screws and not the phenolic top as the vacuums are pretty weak, and then we do 4 passes at 0.0338" to a total cut depth of .1352" to cut through the 1/8" sheet. When we are cutting an entire 4x8 sheet of parts the cut program is anywhere from 5 - 7 hours long and typically after about 3 hours we start having issues with the endmill gumming up and welding to the material and then snapping off, usually run through 3 or 4 1/8" endmills per sheet..

So in an attempt to speed things up we switched to using 1/4" 3 flute endmills. We are still running at the same 18,000 RPM and can run at 25 IPM now and only need to do 2 passes at 0.0675" depth to a total cut depth of 0.135". This has reduced out cut times by almost 60% so now instead of a 5 hour cut program it is 2 - 2.5 hours which is much better! And the machine sounds really good when its cutting at those settings. But now the issue is that although the endmills aren't snapping off anymore due to their diameter, they are still welding to the material and we are still going through 1 - 2 endmills per sheet.. What we found is when cutting with the 1/8" endmill we can run with a very fine mist of Kool Mist and can drop the air line pressure to about 75PSI and it cuts good for about 2 or 3 hours before encountering issues usually, with the 1/4" endmill we have to run the air pressure at 90+ PSI which means our 60 gallon compressor is now running 100% of the time, if we drop the pressure to 75 PSI it gives the compressor a break but we found the endmill lasts longer at 90 PSI, and we have to spray a much thicker mist of Kool Mist to keep the endmill cold enough (probably 4 times as much) and now we are drenching the MDF spoilboard at the cut and having to resurface it every day when we want to use the machine. We did find that spraying some wd40 while babysitting it would help, but it still eventually gums up and wrecks the endmill.

So one thing we did notice is that the issues come either when it starts a new cut, or when its doing the last cut, typically after a tab but not always. We are getting a very thin circular "plug" that sticks to the bottom of the endmill and when it lifts up to travel to the next cut and then goes to plunge into the new cut, if that plug is stuck to the bottom it sometimes will immediately gum up but usually starts cutting good. And the same with the last cut when we are doing tabs sometimes it will drop down after the tab and immediately gum up. I suspect this is the same issue with the 1/8" endmills most likely but they're pretty small so it is a little difficult to see if the plug is stuck to the bottom right before it gums up whereas we can clearly see the thin plug on the 1/4" bits when it lifts up or is running the last cut.

So, sorry about the long story here. Hopefully I have included enough information that someone can tell us what we might be doing wrong or how we can optimize our set up to be able to walk away from the machine and let it cut until done. From all the reading I have done it seems like 5052 aluminum is problematic compared to 6061 but almost every part we cut gets bent so 6061 wont work for us. And I know the MDF spoilboard is not ideal when using a misting nozzle, I am just not sure what else we could use instead? I read that expanded PVC works? We do use the Phenolic top when we cut foam, but we don't have any issues cutting the foam, so if we could keep the MDF spoilboard that would be ideal so we don't have to change out the spoilboard when switching from aluminum to EVA foam, but we might have to get 2 different spoilboards going? Or route out pockets on the underside and put holes through so the vacuum works through the expanded PVC (or other material?).

Perhaps someone knows of a endmill with a coating that works really good with 5052 aluminum? Maybe drop down to 2 flute, or single flute? maybe we should be running faster, slower, slower rpm, need more air, different cooling system, etc etc..?

Anyways, if we have missed any important information please ask below, Thank you very much! I will be cutting today so I will see if I can get any pics that might help.

[FickFab]

Little update for anyone that runs across this. We ended up finally speaking with someone local that had some knowledge on this at a small shop we had never heard of, and she recommended we make the switch from 3 flute endmills to a single O flute ZrN coated endmill. So we picked up an Amana 1/4" Single O Flute endmill (pricey) but in doing so we were able to lower our air pressure to 75 PSI so our compressor is no longer running 100% of the time, we are able to turn our mist right down to virtually nothing.. just barely enough to make your finger slightly damp if held in the stream of air. And we are now running as per below.

5052 aluminum sheets with a 1/4" single O flute Amana endmill at 6IPM plunge, 25IPM feed, 18k RPM, 0.065" DOC, and are getting a 0.0045" chip load. The chips are coming off hot, the tool is cold the the touch after 2 hours non stop cutting, we are able to walk away from the machine now and do not have to worry about the endmill plugging up! Now the only concern is breaking the endmill as we have gone through 2 already (1 our fault, maybe both) and they are rather pricey!

On the note of the endmills, if anyone has any experience with Amana endmills. The exact endmill we are using is the Amana 51480-Z, we purchased 3 of these at a cost of $75/each (compared to $17 each before for the 3 flute...). We ended up breaking one of the Amana endmills in a piece of 3/8" aluminum which was just a stupid mistake where we forgot tabs on a piece and it got loose and snapped the endmill when cutting through. But when we swapped the endmill to another brand new one, we went to cut a sheet of 1/8" 5052 aluminum as per the settings above and the second this 100% brand new endmill touched the material on the very first plunge the very tip of the tool broke off and it immediately gummed up and was ruined. We swapped to the last new endmill we had purchased, restarted the program with no changes, and it went on to cut 3 more sheets after that sheet as well without any issues and is still in use today. So 1 out of 3 Amana endmills having what I can only determine as a manufacturing defect seems like really bad odds. We tried to reach out to Amana to gain some insight and they recommended we change our settings to 12k rpm, 30IPM plunge (ramped), 60IPM feed, and .250" DOC. Our machine will not be capable of running these settings as it is a lighter duty machine, and I feel like 30IPM plunge and 60IPM feed at a lower RPM just sounds really fast? The settings as mentioned above that we are running we basically started at 18k rpm as that is what our machine maxes out at, we started at 5IPM plunge and 10IPM feed and used our over ride until the machine started to get a vibration cutting at 30IPM feed, so we found 25IPM was a good feed rate and the chips were coming off at .0045" which is perfect as per the Amana chart, and then just found that 6IPM seemed to be a good plunge rate, not entirely sure on this though. We do a straight plunge to .065" DOC and I am just not familiar with what a good plunge sound should be. Anyways, if anyone has anything they could chime in with on this I would be interested in hearing. This is a learning curve for us and any feedback is appreciated! Thank you

[mactec54]

Little update for anyone that runs across this. We ended up finally speaking with someone local that had some knowledge on this at a small shop we had never heard of, and she recommended we make the switch from 3 flute endmills to a single O flute ZrN coated endmill. So we picked up an Amana 1/4" Single O Flute endmill (pricey) but in doing so we were able to lower our air pressure to 75 PSI so our compressor is no longer running 100% of the time, we are able to turn our mist right down to virtually nothing.. just barely enough to make your finger slightly damp if held in the stream of air. And we are now running as per below.

5052 aluminum sheets with a 1/4" single O flute Amana endmill at 6IPM plunge, 25IPM feed, 18k RPM, 0.065" DOC, and are getting a 0.0045" chip load. The chips are coming off hot, the tool is cold the the touch after 2 hours non stop cutting, we are able to walk away from the machine now and do not have to worry about the endmill plugging up! Now the only concern is breaking the endmill as we have gone through 2 already (1 our fault, maybe both) and they are rather pricey!

On the note of the endmills, if anyone has any experience with Amana endmills. The exact endmill we are using is the Amana 51480-Z, we purchased 3 of these at a cost of $75/each (compared to $17 each before for the 3 flute...). We ended up breaking one of the Amana endmills in a piece of 3/8" aluminum which was just a stupid mistake where we forgot tabs on a piece and it got loose and snapped the endmill when cutting through. But when we swapped the endmill to another brand new one, we went to cut a sheet of 1/8" 5052 aluminum as per the settings above and the second this 100% brand new endmill touched the material on the very first plunge the very tip of the tool broke off and it immediately gummed up and was ruined. We swapped to the last new endmill we had purchased, restarted the program with no changes, and it went on to cut 3 more sheets after that sheet as well without any issues and is still in use today. So 1 out of 3 Amana endmills having what I can only determine as a manufacturing defect seems like really bad odds. We tried to reach out to Amana to gain some insight and they recommended we change our settings to 12k rpm, 30IPM plunge (ramped), 60IPM feed, and .250" DOC. Our machine will not be capable of running these settings as it is a lighter duty machine, and I feel like 30IPM plunge and 60IPM feed at a lower RPM just sounds really fast? The settings as mentioned above that we are running we basically started at 18k rpm as that is what our machine maxes out at, we started at 5IPM plunge and 10IPM feed and used our over ride until the machine started to get a vibration cutting at 30IPM feed, so we found 25IPM was a good feed rate and the chips were coming off at .0045" which is perfect as per the Amana chart, and then just found that 6IPM seemed to be a good plunge rate, not entirely sure on this though. We do a straight plunge to .065" DOC and I am just not familiar with what a good plunge sound should be. Anyways, if anyone has anything they could chime in with on this I would be interested in hearing. This is a learning curve for us and any feedback is appreciated! Thank you

I would say you still don't have the correct End Mill as you should get a very long life from just cutting the aluminum sheet, those cutters are overpriced for what you are getting

You should speak to this company as your lube is some of your problem also, https://unist.com/pump-warranty.html

[joeavaerage]

Hi,
I had very good success with Di-Boride coated tools from Harvey Tools....expensive but it ended the sticking swarf problems, that was with some rather sticky 5083.

Most coatings like AlTiN and so on are trivalent....but aluminum is a trivalent metal and shows affinity for trivalent coatings....not good. Di-Boride is quad valent and is as
'greasy as a butchers prick' in aluminum.

Mostly I use uncoated tools and plenty of flood cooling, but that wont work for you. The major thing is to get the chips out of the cutzone, using air or flood does not matter, but
recutting chips will result in Built-Up-Edge every time.

Craig