CNC tooling: What's the best?
Here are some details:
We are using 3/4" MDF for a spoil board. Is this best for hold-down?
I would use a solid carbide up and down shear for a clean cut. As for the bit lasting, my guess is that you are cutting too slow. I run at 400 inches per minute, 18000 rpm, and will go faster when patterns and hold-down allow it. We push it as fast as possible until cut quality or accuracy goes down.
You also may want to look at your MCP. We have found that there are different grades of MCP (the color layer is thicker). When we cut the lower quality MCP we need to slow the router feed speed down and change bits more often.
We have been using diamond compression bits with good results. The only time we use solid carbide spiral bits is when we get lower quality MCP.
One of the key issues a rep from Onsrud went over with me was collet care. I now have a set of brass collet brushes that I use to clean the collet with every bit change. Also, once a bit has slipped in a collet, take a VERY good look at the collet. If there are score lines from the bit slipping, then unfortunately, it's probably best to dispose of the collet.
In addition to cleaning the inside and outside of the collet with each bit change, we also clean up inside the spindle taper and the collet nut threads as well.
Since adding this routine I've only had bits slip on 2 occasions, and in both I think I didn’t tighten the nut enough. Before this, we were breaking almost everything that went in the router. There were a few other changes we made with regard to feed rates etc., but collet care was a major change in my procedure.
You wrote that you were using ½” bits. You also listed 10mm spacing between parts. I assume you mean that you are leaving 3/8” greater than the ½” diameter of the router bit or 7/8”. This by itself would not cause all of your problems, but it could contribute. I have tried running only five-tenths of a millimeter larger that the bit diameter, but if a small part got bumped a small amount, the tight kerf caused problems when the small part got bumped into the path of an uncut part. At present, with a straight entry, I run a bit kerf that is equal to the diameter of the router bit plus 2mm. If you are running more than this then you’re causing your router bit to cut more material than required and this will cause the bit to dull quicker. If you were to try and run a kerf the exact size of the bit diameter, I think that would cause some chipping, also.
I also found that when using compression bits, once the bit got halfway through it’s useful sharpening cycle, it began to chip an area about ¾” long at the entry location. This was caused by the compression bit, as the part of the bit with up-cut shear angle penetrated the surface of the board. One thing we are expecting in the next release of Cadcode is an entry routine that not only ramps in on the z-axis but also enters on an angle in the x, y plane. For this entry routine there will be a required bit kerf equal to the diameter of the bit, plus 3mm.
If the brand of post processor you’re using does not allow for an entry routine that is on a ramp in, and you are using a plunge cut entry, this can take its toll on the router bit. This type of entry will cause a dwell point on the part being cut and cause unnecessary heat for the router bit. It will also cause problems over time for the router spindle bearings. What entry speed are you using for your router?
I run a larger router motor than you are running but have been told that the 10-½ hp motor you are using is sufficient. I am running most of what I do at the same 18000 rpm you are running at. Do you know for sure that your router motor and what it attaches to and slides on are not deflecting at faster feed speeds?
I tried the diamond tooling but after two sheets I knew it couldn’t work for the speed I was looking for. The diamond bit I tried had almost no shear angle on it. I was told to use a feed speed of 350 inches per minute. At that speed, with a brand new bit, I was causing parts bigger than 12” x 12” to move, and I have a 40 hp vacuum pump on my router. I sent the diamonds back after two sheets.
Before the diamonds I used ½” solid carbide compression bits. They were no-name brand “deals” and they each cut 35 sheets of 5 x 8, ¾” thick Canadian core melamine 2 sides. While running my first compression bits I was in the process of getting the post processor working with my router. I was also running at feed speeds under 600 IPM. At that time I also had to do complete stops on inside and outside corners and at any time the bit changed locations in the z-axis. Even under these less than ideal conditions, these 2 fluted ½” bits cut 35 sheets each.
After the diamond experience I called Vortex Tooling. Based on a feed speed of 1000 IPM and 18000 on the router motor, they suggested a two-flute compression bit. I ran two of these bits at 1000 IPM and cut more than 45, 5 x 8 sheets with each bit. When I tried to go up to 1200 IPM, the bit started chipping immediately. As long as I stayed in the 900 to 1000 IPM, the bits ran great.
After running the two flute ½” bits I ordered two 3/8” triple flute bits from Onsrud. Using these bits I was able to run at 1200 IPM. At this feed speed I began to see some chipping on the top surface, at 18 sheets. I dropped backed to 1000 IPM and the chipping stopped. I ordered two more of these 3/8” bits and when I started running the third one of these bits, it broke on the tenth sheet, running under ideal conditions. I was cutting at 1000 IPM and it just snapped flush with the nut on the tool holder. Since I broke the 3/8” bit, I have learned several additional details about these bits and tool holders, so I haven’t given in on 3/8” bits. Vortex is going to produce these 3/8” triple fluted bits in the near future.
The smaller diameter bit we can use is going to be easier on the router motor, allow for faster feed speeds, make it easier for the vacuum to hold down and make less saw dust. If breaking continues to be a problem, I am going to switch to triple fluted ½” bits but I have several different things to try before I go to those bits.
It helps to have only the minimal amount of bit sticking out of the tool holder. At this point I will have to change a setting in my control that will give me additional stroke in my z-axis. Onsrud is supposedly working a compression bit 7mm in diameter. By shorting the bit, the smaller diameter bits may be the way to go.
I think that most people running routers similar to yours or mine for nested production will agree that compression bits are good for at least 45 sheets of ¾” material cut into average size cabinet parts. How much faster and how many more sheets of chip free cutting may depend on your router, and how a post processor drives it. My router before it had the ability to run at high speeds through corners and while changing direction in all three axes’ at the same time is the best example of this. The stopping and starting in corners and running at less than 600 IPM was not what the 2 fluted ½” compression bit was looking for.
The other thing you need to look at related to your 8 to 10 minutes per pattern times is drilling. If you add up the cutting inches in an average pattern, you will find + or – 1500 inches. You can do the math and see that whether you are running at 500 or 1000 IPM, the cutting time makes up only a part of the time that a panel is on the router. When I have a pattern with many small parts that require tabbing, the tab cleanup time can be as long as the time it took to cut the entire pattern.
Some router makers are offering limiting drill head configurations. For my needs I decided that I wanted at least 5 spindles in the x-axis and 8 spindles in the y-axis. I keep 5mm bits in each of the spindles in the x-axis and in 5 of the spindles in the y-axis. Then in my design packages I set them to put five 5mm holes everywhere there is an adjustable shelf. With my drill head configuration I know that no matter which way a cabinet side gets turned in the nested pattern, when an adjustable shelf is called for, the drill head is only going to go down one time. Several of the machines I looked at with limited drill head configuration would have to drill these five holes one at a time. Drilling one hole at a time killed my per pattern times.
The other issue related to drilling is how well your post processor optimizes drill moves. At shows I have seen drilling on patterns that made no sense at all. The drill would be at a location using a 5mm bit and then for the next hole it would move five feet away and drill another hole. Cadcode starts drilling at one end of the 8’ panel and traverses back and forth in the x-axis. As it travels in the y-axis it never causes the machine to back up in the longer y-axis. Your post processor also should optimize tool changes. Cadcode does all drilling first. Then it does any routing that falls on the nested parts and finally it cuts the nested pattern. This sequence keeps the tool changing to a minimum.
With my configuration running at 1000 IPM, my average pattern time is between 6 and 6 ½ minutes. For cutting particle core melamine, solid carbide compression bits are what most people I talk to are using. I would suggest starting with triple flute ½” bits and trying to eliminate each of the issues I listed above as the cause of your chipping problem. What works for me at 1000 IPM on my Northwood router may not work for you on your Rover. Since you are cutting 5/8” thick material there is no reason that you should not be able to cut at a feed speed of 1000 IPM and get at least 50 sheets of chip free cutting before sharpening your router bits.
Is your router sitting on all of its leveling points firmly and is it level?
Are you getting any deflection within the router slide table or whatever it slides on?
Is your post processor instructing your router to cut in a way that minimizes stress on router bits? Entry speeds of 3500 IPM, ramping entry instead of plunging entry, no stopping on inside and outside corners?
Are you cutting in the proper direction? For a router motor spinning clockwise and cutting nested parts, then you cut traveling counter clockwise around the part.
Do you have the router bit protruding out of the tool holder the least possible amount for your router?
Is the tool holder you are running your nested bit in undamaged? Are you following the tool holder care procedures listed previously?
Are you leaving a bit kerf equal to the diameter of the bit plus 2-4 mm of additional space?
Have you checked the router motor\spindle to make sure it is spinning true?
The collets are the most important part of the process. They should be changed 3-4 times a year minimum, more if the machine is being run 3 shifts or if it has crashed.
Are you using a mortise compression bit? This is the compression that has the short up-cut on the bottom. This helps with drag and cutting into the spoil board too much.
Are you having any movement in the parts? What size of vacuum are you running? Have you resurfaced your spoil board to make sure that it is flat and true?
Have you checked the run-out in your spindle? I have seen new machines with .005 to .010 run-out. Run-out is the amount the spindle is running out of round. This is checked by placing a round rod that you know is true in your spindle. Then place a dial indicator on the spindle and turn the spindle round to see what kind of run-out you have. Run-out is usually from worn bearings in the spindle if you have new collets.
We have the 3 flute compressions or 3+3 but the feed rates that you must run for this tool are very high and hard on the machine, also.
The comments below were added after this Forum discussion was archived as a Knowledge Base article (add your comment).
Comment from contributor A:
Would you like to add information to this article?
Interested in writing or submitting an article?
Have a question about this article?
Have you reviewed the related Knowledge Base areas below?