PDA

View Full Version : Complete Newb Looking for guidance



wrenchdoctor
12-30-2013, 03:58 PM
Greetings folks.

I am hoping you can help me gain some understanding and knowledge with something at work that I have been increasingly involved with troubleshooting. Here is the backstory :)

I work at a packaging company as as the IT tech.I have a maintenance background, and they ask me to help with most anything that has no "person" to deal with. Some days its locating replacement parts for a 50 year old machine, and some days its hanging/wiring lighting. Whatever is needed, I generally take care of and welcome the challenge of the day. One of the areas that I have been asked to help out in is of the CNC router we have. There were a couple electrical problems with it when I started, that I was able to repair and get the machine functional again, and in the process I couldn't help but notice the ignorance of the operator/s. Nobody really knows the machine, they follow some printout that someone arbitrarily made and that is how they run everything.

The machine in question is an AXYZ 5010. They employ a designer who makes the design on a CAD program, exports the design to Router Type 3 CAM software, where it is "cleaned up" and exported to the CNC machine as an NC file. Somewhere along the way, between designers leaving, operators moving on, all of the training has been lost and there is only the bare minimum of knowledge. All of the work thus far is usually on 3/4" CDX, untreated 2x4, and 2x6. The designs are very simple, as they are generally cradling a part or piece inside a crate. One that comes to mind is a 3ft 2x4 with 8 round holes cut right up the center.

Before I got involved, They were cutting this example above with an Onsrud Upcut (52-367) 1/2" bit.They were cutting 1.57in deep at a feed rate of 50in /min. 16,000rpm. One pass, project complete. The problem, is that they were killing the bits at an unethical rate (bit toasted after 6 2x4's). Again, no training, they saw this as the norm......

After a lot of online research, I found out more and more of the answers I was after. Chip load was the culprit, and I tried several things to make the bits last longer. I have been largely successful, increasing the bit life to where they have replaced one bit in the last 3 months (200+ projects). Now, they cut the project above with the same bit, running 21,000rpm, .525 deep at a feed rate of 350in/min.

After doing a project, immediately after the spindle comes to a stop, I feel the cutting end of the bit and it is for all intents and purposes, cool. I can feel a faint amount of warmth. As the machine cuts and ejects the chips, they are warm.

Is there anything else I can do to optimize the production of this machine? looking around at some of the other posts, I see people are cutting quite a bit faster. Should I go to a smaller bit? Higher or lower RPM? Stick with what I have and use a higher feedrate?

Is there an approximate size of the chip I should be looking for that would be indicative of a good chip load? Right now I am getting shavings akin to sawdust. Seems like there is more efficiency to be had.

mmoe
12-30-2013, 04:58 PM
There are different strategies that you can use to optimize feedrate, but they may not have a net improvement to the overall time taken to process. For 2x4 pine type material, my biggest concern would be movement of the material both by way of vibration and the unstable nature of the material itself. A couple of thoughts might be that the method to hold down the material may or may not be ideal. Are you just holding it in place with screws at each end of the board? If so, there is likely a lot of movement of the material due to deflection/vibration that will limit what you can do with any degree of reasonable finish quality. Are these parts that get made generally the same way every time? If so, a vacuum fixture to hold the material down hard will potentially allow for much higher feedrates with good finish results. Fixtures like this can be time consuming (a couple hours) to build, so if it's just a few parts, it just won't make sense.

You could also use pocketing to cut the holes in your example, which while taking more linear distance of motion may allow for higher feedrates with good results. I'd probably employ a spiral pocketing in two passes to create a hole through a 2x4. The thing is, if you only use .5" of the cutter from the tip, you are going to wear out the bit faster than if you use 1" of the cutter. In order to use 1" of the cutter, you need to get the cutter so that it's not buried all the time. By starting from the center of the hole and spiraling outward in say 1/8" steps 3/4" deep (two passes making up 1.5"), you could probably run at around 300 in/min with 2 passes instead of 350 in/min with 3 passes. The spiral will take a bit longer than just cutting a circle, but it will be made up for in the reduced number of passes. The bit will be utilized better since you are using more of the cutting edge at all times.

All that said, 3 months is not a bad amount of longevity from the bits. Depending on what I'm cutting, I've had some jobs where you go through a bit in a couple of days, but that's also producing hundreds of parts and running 8-10 hours per day. I think that you should start tracking longevity by hours more than projects, since projects is a more subjective concept. If you are running at 16,000 rpms, and you run a bit for 30 hours of actual cutting time on a 2 flute bit, you can figure that each flute has made 28.8 million cuts. If you get more time the next time that you can attribute to a change in your proceedures, you can quantify how much of an improvement you've made based on how many more turns you're getting out of the bit.

There are other factors that are harder to gauge, like how much time are you in rapid or plunge/retract situations vs. side cutting at feedrate, but they do need to be considered. For example, running a spiral like I suggest will keep the bit engaged just on perhaps half of the circumference that running a profile where the bit is buried. I think that it's likely that the result will be cooler operation and higher possible feedrated during the motion. The other result is that there will be less time spent in rapid, plunge or retract, since you are only making 2 passes vs. 3 passes. It would be an interesting comparison to see if having a higher percentage of time engaged to the material in a more ideal manner (spiral) actually increases longevity vs. burying the bit and cutting more air in rapid, plunge and retract. I have a feeling it will, but I don't think you'll know until you test this with actual numbers. The bits may be cutting more in the spiral condition, but perhaps cutting in a more ideal manner will extend the time that the cutting edges remain sharp. On the other hand, being in contact with more material may also result in dulling those cuttering edges faster regardless of how ideal the chipload may or may not be. I tend to think that burying the bit (full width passes) likely results in premature wear, but I don't have hard data to offer, just ideas on things to try.

As for chip size, I find that it's much the same as a table saw type chip, perhaps even a whisker smaller. The faster cutting rates you are seeing are likely for MDF or partical board 3/4" sheets. For a sheet of melamine particle board, for example, I find I can run close to 800 in/min at a full 3/4" pass with a 1/2" 4 flute bit running around 15,000 rpms. I prefer to go a little slower as I find I get a better finish for an edgebander at 400-600 in/min, but that's more about quality of cut than what "can" be done. I suspect that you "can" cut up to 1000 in/min with the head running at full speed (20k rpms), but I don't like pushing my heads that hard as I think it wears them down faster. I go about 25% slower through MDF and plywood (baltic/russian birch core for example) and while CDX is not very hard, I'd probably go about the same for that as well as I suspect it would splinter a bit (300-450 in/min). I'm often cutting at around 10,000 mm/min, which is just a bit under 400 in/min.

ger21
12-30-2013, 07:36 PM
You can probable drop the rpm down to 15,000 and still cut at 350ipm. I've been cutting hardwoods the last 2 days at 500ipm and 16,000 rpm with a similar downcut bit. Personally, I would never run a 1/2" tool over 16,000-17,000 rpm. You'll just burn them up if you do.

You also might want to try a chipbreaker spiral, which will let you cut even faster at the same rpm. You can probably go up to 600-700ipm at 16,000 rpm.

wrenchdoctor
01-03-2014, 09:05 AM
mmoe, thank you very much for all the information. I found it to be quite helpful and I will put some of this expertise to work and see what happens. Sorry for the slow reply. With the New Year Holiday, I was a little busy with work on my first day back from the holiday and I couldn't reply in a timely manner.

The Table has vacuum for hold down, and originally, we were screwing the lumber down to the spoilboard to keep it in place. As you eluded to however, the board was moving, and I was seeing some vibration. Since this is a more production based run, that we do on a regular basis, I elected to create a jig. I asked our CAD guy to make the outlines of the projects onto a piece of CDX, so that the 2x4's would fit within the confines of the CDX tightly. Then we screw the 2x4's into place. This seems to have taken care of the vibration and movement. I went back and had jigs made for all of the regular runs that we do. They were previously cutting one at a time, and now they are doing 8-12 at a time depending on the size of material being cut.

The CAD guy makes all of the toolpath decisions, and he is very frustrated with the Type 3 software due to its lack of intuitiveness. He's only doing what he knows, and really hasn't branched out. I have watched him a few times, and I will get him to do use spiral pocketing on the next new project. I didn't think only using .5" of the bit would lower the bit life. I know I was not using much of the cutting edge at all, but I was afraid that taking alot of material out and overloading the bit. I will go to a two pass method and slow down to 300ipm like you suggested. I was actually thinking of lowering the ipm anyhow because when I calculated the chipload, I was at or near .033 if I remember correctly. At least one "rule of thumb" I came across for wood was no more than a .025 chipload. However, even with such a high chipload the bit still stays cool so I dont think I am hurting it.

Thank you for the suggestion on the hour mark. They had always said they replaced bits after "X" number of boards, so I just ran with it when I started. Hours is certainly more accurate and I will get the operator to log the hours on the bit in the future. As for the change in strategy on bit cutting, I will try and use the spiral method and deeper cuts for a while and see how that effects bit life. I will try to quantify any changes as my observations add up and report back. That is going to be something that will be more of a soak test. The operators are more than happy to see the machine running so much better and with no trouble, and they are pretty eager to try and make things even better. My biggest issue will be the CAD guy and his frustration. I have been looking for information and help to aid him, but there isnt much to be found. I suspect that Router Type software does not have a big market share and that is why there is very little information to be had.

Thank you for the info on the chip size and speeds. With the setup I explained in my OP, we have never had any splintering whatsoever. The way they were doing it previously gave them some odd looking cuts though. I suspect that was due to vibration, movement, too slow a speed dulling the bit prematurely. I am all for not running the head right at its limit.Especially since it will be me having to make all the repairs LOL.


ger21 - I don't know what I was doing lol. I just read on the motor that it was capable of 24000 RPM so I elected to run it at 21000RPM to keep it from running at its limit. I looked around and was unable to find any max. RPM on the bit so I ran with what I had. I will be slowing it down to 16000RPM just to be on the safe side.

As for the bits, I looked into the differences on them and had elected to replace our stock (when we run out) with some compression bits. Since I don't plan on cutting 1.5" deep anymore, I think a 1" cutting surface bit would be the better choice as they are cheaper. It is my understanding that the compression bit gives the clean edges of the downcut, with the clearing ability of an upcut. Is that correct?
If the chipbreaker spiral is not a compression bit, would you mind elaborating a bit or perhaps provide a link where I'd be able to shop for them?

Thank you very much for all this wonderful information. Its nice to have some corrective advise and some input from the pro's. Im very appreciative.

ger21
01-03-2014, 10:52 AM
A general rule for wood is cut as fast as you can (highest chipload) until either the bit breaks, or the cut quality is unacceptable. The higher the chipload, the longer the tool life.

For what you're doing, I'd run the tools as long as they keep cutting OK. As they dull, they'll get louder, and the cut won't be as smooth, but you can probably run them a lot longer than you are. THey should be good until there's noticable wear on the edge of the flute. We cut a lot of melamine sheets, and we can still get good cuts with a visible groove worn into the edge from the melamine. This requires more material to be removed when sharpening, so they can be sharpened fewer times, but we use them longer. It's a bit of a tradeoff.


A compression bit will act a lot like a downcut if you're not cutting through in 1 pass. The bottom upcut portion is typically rather short, and most of the upper portion of the bit is a downcut, so it acts like a downcut, and won't remove a lot more chips then a downcut.

If you can get away with a "rippled" edge, then you might want to look at a roughing bit, which has a sort of serrated edge. They can cut at incredible speeds, with much higher chiploads, and they are a lot quieter.

Take a look at Vortextools.com and look at their standard wood bits.

mmoe
01-03-2014, 11:26 AM
I also recommend Vortex tools. I've used them for years and they just seem to be slightly better than anything else I've used, which includes Leitz and Onsrud among others.

wrenchdoctor
01-14-2014, 07:57 AM
Hello, I just wanted to check in for an update. I have not had to do anything with the machine lately as business is slow. I am in the process of trying to find one of our previous employees to show me the ropes on the CAM program we use here. Once things start to pick up I will try the things you guys have shown me here. Its funny you mentioned the Vortex bits, because I was actually looking at a Vortex Compression bit just recently and was leaning toward them. Thank you very much

wrenchdoctor
01-14-2014, 09:04 AM
I must have spoken this into existence this morning, because as soon as I replied to the post and went out to carry on my business, I was handed a file to get to work on. With no previous training or experience with these programs or even CNC in general, the learning curve is steep to say the least. I feel like once Im off the ground and familiarized with the programs, I will be OK. With that said, I have some more feedback/questions......

1- Chipload - I downloaded this handy dandy chipload calculations spreadsheet from another post somewhere on this forum, and according to those calculations, In order to achieve the recommended chipload of .025, I'd need a feedrate of 600, and spindle RPM of 15000 with my 2-flute bit. The operator is pretty sure that they have done something very similar to this in the past and the spindle actually got bogged down and they had to stop for fear of damaging something (granted, I've made some repairs since then, namely on the servo controller wiring.) but that, to me is a red flag. I suggested that the bit may have been dulled but they are sure it was new. For the time being, they are cutting the file in question at 200ipm, 21000rpm, 1" deep. When I learn how to edit this in the CAM program i will work my way toward this chipload.

2- Probably a dumb question, but in all of these calculators I am seeing for chipload, the actual cutting depth is not a factor. How is that possible? The amount of material the bit is exposed to does not factor into its chipload. I am having trouble comprehending that.

Today, I am going to be involved with cutting a project that does have a schedule that will allow me to play around a bit, so it is my intention to try a few different strategies. For whatever the reason, the maximum feedrate is set at 500ipm. I dont know if that is a setting that is controlled by the CAM program or what, but I seem to remember reading somewhere in the literature that the table was capable of 1500ipm.

ger21
01-14-2014, 09:23 AM
A chipload of .025 will probably require a 10HP spindle. If you have a smaller spindle that can't handle it, lower the feedrate.

As far as depth of cut, with a 1/2" bit, I start to lower the feedrate when depth of cut get's over 3/4". I'll drop it about 15-20% for each additional 1/4" depth. I probably wouldn't cut much deeper than 3/4" per pass, though. Cutting deeper will put even more load on the spindle.

wrenchdoctor
01-14-2014, 09:54 AM
218650
I attached a pic of the Spindle motor (I think, lol). It looks like I am only at 8.9HP.

Until I can successfully change the files settings, we are stuck doing it this way. I went out there a few minutes ago and right after a cut of 6 pieces of OSB (2x 1/2") the bit was a little warm, I slowed the speedrate down from 200 to 150ipm and will recheck in 10 minutes.

The guy who was doing all of the CAM/CAD work has been relieved of his duties, so I am up a creek for now.

ger21
01-14-2014, 10:04 AM
150-200ipm is way too slow. Depending on depth of cut, you should be cutting at least 500ipm.

WHat rpm are you running at?

You should have plenty of spindle power for any speed you want to run at.

wrenchdoctor
01-14-2014, 10:09 AM
OK, Thank you very much. The next cut will be at 500ipm, and I'll report back.
RPM is set at 21000. All I can change right now until I learn the ropes of the CAM is the feedrate. I am WILL get the RPM down around 16,000 as suggested earlier in this thread.

and before I forget to say it, Thank you very much, I do appreciate all the help so far.

mmoe
01-14-2014, 10:12 AM
Looks like that spindle should be fine to me. 8kw is still a pretty solid spindle. The bit will get warm and I've had the chips coming off the table be quite warm as well, I'm not sure you can really take a whole lot from that. I'm not sure of the exact temperature, but I suspect that a carbide bit can reach 300 degrees pretty easily and not loose it's hardness. Until it reaches that point where the bit is starting to loose hardness, it should be fine. If your material is held down well, I can't see how you wouldn't be able to cut 1/2" OSB at 400ipm at the least with a 1/2 inch carbide bit of decent quality.

ger21
01-14-2014, 10:28 AM
I agree on the heat. If it's too hot, the bit will be dark brown or black on the end. If the bit is not changing color then it's not too hot.
I've read that even at high chip loads, temperatures at the cutting edge can reach many hundreds of degrees.

One thing to consider is to watch for pitch or resin buildup on the bit. Cutting construction lumber can cause a lot of buildup, which can then generate a lot of heat. If you see any buildup on the bit, get some bit cleaner and clean the bit's daily, or even more frequently if needed.

wrenchdoctor
01-14-2014, 10:39 AM
218664218666

Here are a couple more pictures. One of the dust coming off of the cuts, and the other one of the "jig" used to hold the project in place. There are also screws in place as well. As you probably already know, After the cutting was done, the bit was roughly the same temperature as it was on the slower passes. I did notice that the chips coming off of the bit were noticeably hotter.

Thank you for clearing that up for me on the bit temp. I was so preoccupied with the temp of the cutting edge. I was under the impression that anything more than warm to the touch is bad. Pretty unreasonable, I know, but its all I had to go on. There is absolutely no discoloration of the bit as of yet, and no buildup of any kind. I told the guy doing the operating to be on the lookout for it though

Correction on that spindle speed by the way. For some reason, it has been bumped to 23000rpm, I had previously asked the CAM guy to not go over 21k. Apparently, something got miscommunicated.

wrenchdoctor
01-14-2014, 11:00 AM
Alas! I opened up the NC file and edited the spindle RPM to 16000. I was trying to do that earlier, but in the wrong file location. Our CAM program outputs the NC file to folder A, and we move it to the folder B, which is on the tables controller. Well, I edited it in folder A but forgot to copy it to folder B..... easy enough fix. I'll figure out how to do it in the CAM program later :)

wrenchdoctor
01-14-2014, 11:13 AM
Maybe its just because I have never heard it do this before, but at 16k, the board wants to lift pretty bad, and the spindle does appear to get slowed down/bogged @500ipm. The noise coming off the machine is definatly more labored, where as before, at 23k, it was zipping right through. Good, bad, or indifferent?

ger21
01-14-2014, 11:34 AM
By lowering the rpm, you increased the chipload by 30%, which probably increased the cutting forces even higher. This will also cause a noticable difference in cutting noise. At high chiploads, big spindles like that can create a tremendous amount of force.
I wouldn't expect what you're doing to be able to slow down that spindle, though.

How deep are you cutting?

You might also want to consider downcut bits, to prevent the lifting.

wrenchdoctor
01-14-2014, 12:09 PM
I think what I am likely hearing is the spindle loading up. I will do it again to see if it is actually slowing down. It might just be the higher load and I've just not heard it before. I am cutting right around 1" deep. The operator kind of panicked cause he'd never heard it do that before. We are all inexperienced though.

When it is time to re-order, I am going with a different bit, but I was leaning toward the compression bit due to its characteristics. Should I forget it and go downcut instead? Also, is a 1/2" bit even necessary for what I'm doing? We currently only have 1/2" and 1/4" collets, but I'm sure I could get the company to spring for a few collets.

wrenchdoctor
01-23-2014, 11:57 AM
Hello again!

Another update..... I am now official CAM guy as the design guy was terminated for something pretty stupid not related to work. I am in the process of learning the CAD program and I am ok with running the CAM program. That is to say, I can design the table file, import into the CAM, and create a toolpath to send to the machine. I am not "great" yet, but I am getting the job done and the powers that be are impressed that I have jumped in and taken the reins with very little drop off in output. However, I am getting better and continue to push. With that said, here are a few more questions;

I have implemented all of the changes you have suggested since the original post, with the exception of the new bits, and using the spiraling cut as opposed to cutting out a single piece. Reason for this is I haven't had to deal with any files that include circles, and I cant find the option in my CAM program. The bit is now running 16k rpm, cutting at 500ipm, 2 passes averaging no more than 1/2-7/8" a pass. I am also operating the machine for the time being, so that I can see any mistakes I a making, and learn the whole process better.

I feel like I can go faster than 500ipm while cutting as the spindle doesnt seem to be working hard at all, and based off what you fine folks have suggested. The problem is, the max on the machine is 500ipm. According to the documentation I have for the table, it is capable of up to 1800ipm (if I remember correctly). Is this limit imposed by the tables hardware or is it the CAM program doing this?

In the CAM programs tool database, there appears to be a limit of 500ipm, I have changed it to 1500, but that doesnt seem to make a difference. Also, the RPM was at 23krpm, and I adjusted it to 16K. When I output the NC file after finishing, the RPM is reverted to 23K every time. I have to open the NC file and edit the rpm back to 16k. What gives? Im sure I've saved these settings.

Is anyone familiar with the TypeEdit (Type3) CAM software? That is what I am using. Its an older version, and the company really wants us to buy an update rather than answer questions we have regarding problems we are having. For the price they quoted, I think there are cheaper options that I can explore as I am doing what I would consider to be very basic type work with the table. I've seen a couple pretty highly regarded programs right here on this forum that I would want to point my company to consider buying, and they were much cheaper.

BuckNaked31
01-23-2014, 12:21 PM
Check your tool database, once you edit the feedrate and spindle speed for that partcular tool, it should post that way every time.

Sent from my SCH-R720 using Tapatalk 2

ger21
01-23-2014, 12:52 PM
Also, if the machine has a tool table in the control, the feedrates set there may override whatever is in the g-code.
If the feedrate and rpm in your g-code correct?