Melamine Tooling Issue: Grooves Worn Where Tool Contacts Paper
From the original questioner:
We have used Rossberg, Funder, and a local brand made in Arlington, TX. We have used Cormatt,, Lietz, Onsrud, Missenhimer, Whiteside, all 3/8 mortise compression. My tooling supplier and other tooling suppliers are telling me that everyone is having the same issue. The material suppliers are saying that they do not know about this. Usually speed rates for this bit are around 18,000 spindle speed with around 650 feed rate.
From contributor K:
You may want to look into DLC bits.
From contributor M:
For a two flute tool you are not too far off in feeds and speeds. I use a 3/8 3 flute at 16K and 1100 IPM for 3/4 in one pass. You may be able to slow the RPMís or increase the feed a little. Do your tools stay bright or do they get black?
Courmatt, Vortex, and Onsrud are all industry standards and excellent tools. For my money I get the best life from Onsrud MW tools, short from Maximum Wear. I believe they do the carbide differently with MW, it is not a coating, although that is available too. Coatings are usually gone after your first sharpening, but they help when a tool is new.
I have found the grooving issue is worst with laminates, way worse with Wilsonart products, and probably least bad in Abet with Formica and Nevamar somewhere in between.
The melamines have not been much trouble for me. I use more Tafisa than anything else, but other brands work into the mix too, especially with all of the LEEDS work being done now. Measuring in number of sheets is difficult since people cut different numbers of parts and have different part densities and sizes, but I cut more than 50 sheets of typical cabinet parts densely nested with one tool if it is all melamine. Mixing up materials is always going to make your tool life less since it is harder to optimize feed rates in multiple materials.
To sum it up, yes I find that the surfaces are indeed harder in the recent past and it does seem to affect tool life. Diamond is usually the suggested solution but I resist diamond for a few reasons. It isn't on cost either but instead on the reality that I will never be able to optimize feeds and speeds for the dozens of materials I cut on a weekly basis so I will never get the tool life I really should. I would also have to sacrifice material yield (diamond is larger in diameter so you have more kerf) and also does not have really good tool geometry (it is hard to make a really slick three flute compression cutter you can sharpen in diamond). If I cut only melamine and p-lam, I might sacrifice some speed and material yield and go for diamond. For now I will keep using the Onsrud MW and hope something even better comes along in high-grade carbide. I am always willing to try a new suggestion.
From contributor Y:
I have been having similar issues as well. With proper feeds and speeds your bits do not burn? Mine are coming out black after little use. I have been trying a mixture of feeds and speeds and things are getting better.
From contributor M:
My bits do blacken after a while; nearly everyone running three flute bits will likely run into this, and to a slightly lesser extent two flute and least with one flute. In a nutshell, the problem is this:
Issue # 1: Heat is the enemy. All tools get dull eventually and dull tools heat up fast.
Issue # 2: The faster your top speed, the more flutes you can use. My particular machine is good for about 1200 to 1600 IPM and that is reasonably fast. I use a three flute tool at these speeds. If your top speed is 800 or 900 you should be in the two flute range, and 300 to 600 likely down toward one flute tools, all assuming roughly 18000 RPM (chip loading permitting) which varies from tool to tool.
The problem is that most of the time machines with a top speed of 1600 IPM are traveling more slowly than top speed since they have to accelerate. Low mass machines that have lower head mass (often bridge gantry) are apt to accelerate more quickly. Heavy mass machines (big iron or overarm) are generally slower. My machine is overarm and heavy. It is solid as a rock, but it takes a long time to accelerate to top speed. All the while it is accelerating the bit is spinning at constant RPLM because the controller (and to a certain extent the spindle) though very reliable is not sophisticated enough to slow down the RPMs into the corners or have the capability of adjusting the RPMs for feed speed. This creates poor feed/speed balancing and therefore faster machines that accelerate slowly generate more heat.
Nearly all machines suffer from this malady to one extent or another. Some machine manufacturers are beginning to address this problem now that machines are getting faster and the heads are heavier with drill banks and aggregates and other options. Controller/spindle combinations that allow for ramping speeds into and out of corners would solve this problem very well. In the end, I slow my spindle down to help alleviate some of these effects but rather than drop speeds and go with 800 IPM and two flutes I live with this imperfect balance.
From contributor Y:
I am new to CNC we have had the machine for about a month now and it gets moderate use. It is "big iron" and capable of cutting at high speeds. I have been experimenting with different combinations.
It is a nesting router and one thing I notice right away is that it is always slowing down (feed) to turn a corner. I nest out of cabinet vision and it eliminates plunge cuts to one at the start. I was told plunging was hard on bits as well. Might I be better to slow my feed and RPM down in the nest so on the corners it is not so fast? I cannot change the feed/rpm within the nest to compensate for corners. My ramp up speed is fast (the installer actually slowed it down) so most of the time it is up to full speed quickly.
From contributor U:
If you program the tool to oscillate while cutting you will reduce the wear line on the router bit. Itís not always possible depending on the type of machine or the type of cutting youíre doing.
From contributor M:
Is XP a different carbide or is it a coating or both? I am not asking for the formula for your secret sauce, just an indication of qualitatively what it is you mean by XP. Vortex offers a particular bit I like, the 3230. It is a three flute compression, but it is made from standard carbide. Onsrud has a similar bit, their 60-125 also in standard carbide, but it is not offered in a MW material. I have been using an Onsrud 60-124MW for exactly this reason, but it is a mortise compression not a standard compression. I really want more up-shear in this 3 flute bit, so if you offer a 3230XP I will be glad to give that a try.
From contributor M:
I think everyone here in this discussion understands chipload and its painfully obvious relationship to feeds and speeds. What you seem to be missing is the equally obvious fact that abrasive material, like Wilsonart laminate and to a lesser extent many other plastics and yes, even melamine surfaces will wear the portion of a tool that comes in contact with it differently than the core.
The original poster has a perfectly legitimate comment. He may very well benefit by dropping his RPMs some or increasing his feed rate a little according to chipload tables. That being said, I have never changed a bit on account of the core area wearing more than the melamine contact area. Look closely at any of your bits that are nearly used up, pull out a microscope (if you can't see it with your naked eye) and tell us all here where the tool is failing.
From Brian Personett, forum technical advisor:
I would echo Contributor M's comments. I think everyone understands chipload. But my experience has been that when you get into the realm of 1/2" and 3/8" router bits, chipload becomes less of a factor. I went through all this many years ago. I had friends who were going through the same issues. We all had different machines and located in different parts of the country. We shared all the info we had, experimented with different combinations and what we found was that no set combination worked for all of us. The guy in NC ended up with Brand X bits, running at X RPM's with X feed rate. I ended up with Brand Y bits, running at Y RPM's and Y feed rate. The guy in CO ended up with Z.
Oscillating Z can help but depending on what you're cutting, chipping can be an issue. As has been pointed out, the router guys definitely have issues with oscillating. I have found that I start a new bit at a certain distance below the material, and with each cabinet I lower it .01mm to be helpful.
There are a myriad of other factors that play into this equation. Southern board, western board, Canadian board, paper weight, laminate brands, different finishes. I know I saw dramatically different results with tool life within one brand of melamine when I used to use Panolam, depending on whether it came out of Norcross or Huntsville. At the time Norcross being southern board and Huntsville being Canadian board. I would also be willing to be bet there were differences in the melamine composition as well. The long and the short of it, are there some guidelines you can start with, absolutely, are there hard and fast rules, in my opinion, no, you need to figure out what works best for you.
From contributor G:
I've been trying a coated tool from Active Machine recently . We cut 75 sheets of board with Nevamar laminate on both faces with one bit, and it was still cutting well when we stopped. It does have a groove worn in it. The groove was pretty small at 30 sheets, but didn't get much bigger at after 75. The cut quality is very impressive. If you run your finger along the top edge, it's nearly as smooth as with a brand new bit. This is nesting on a Morbidelli, so no oscillation was used.
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?