Cutter speeds

Nick M Singer · Post by **Nick M Singer** » Tue, Sep 06 2005, 9:14AM

Anyone got any advice on the correct speeds for cutters especially the main outline tool. I am trying a number of cutters at the moment on an experimental basis. I have tried a Lach disposable diamond 1/2\" at 10 M per minute 22000 rpm. That was apparently wrong and the cutter started chipping after only about 5 or 6 sheets. I then tried a 3/8\" vortex triple flute at 15M per minute at 18000 rpm (Thermwood recommended). This cutter also burned and chipped after only a few boards. I am cutting melamine laminated chip board and MDF. Thanks in advance.

Jody Wilmes · Post by **Jody Wilmes** » Tue, Sep 06 2005, 1:06PM

I normally use a 3-flute 3/8\" Vortex compression tool @ around 400 IPM (10.16M?). I almost always cut @ 18000 RPM's.
I have also used a 2-flute 1/2\" Vortex compression tool @ around 600 IPM (15.25M?) with good results. Same RPM also.
All tooling I use is made of solid carbide. This makes a huge difference in life over high-speed steel.

I have not personally used these tools in production, but have been to companies that have. I've also heard of companies cutting bad material with aluminum/metal chips in the MDF sheets. Not saying this is necessarily your problem though.

I would've thought that the diamond tool would work well for the MDF, don't know about the melamine though. Compression tools are the standard for melamine.

Forrest Chapman · Post by **Forrest Chapman** » Tue, Sep 06 2005, 3:12PM

Hey Nick,

Just our experiance. 3/8- 2 flute comp. For 5/8 mel. 18,000 rpm at 700 ipm. For 3/4 mel. same rpm at 600 ipm. The same should apply for most sheet goods. One thing though is seperate the bits you cut mdf with. They tend to dull faster when switched from one material to the next. The general rule of thumb is to cut as fast as you can without moving parts, breaking bits, or losing cut quality. As a result your bit stays cooler and hence last longer. We can cut on average 80 to 100 sheets of mel. on 1 bit. 30 to 40 of mdf. One other thing we noticed a few years ago are some mel. cut cleaner with a conventional cut not climb cut. I hope this helps you out. Most of this we learned on our own.

Forrest

Glenn Van Reason · Post by **Glenn Van Reason** » Tue, Sep 06 2005, 3:59PM

We have been having the same problem with our bits. Started with feed at 12M per Min and 13,000 rpm, got about 30 odd sheets to a bit. Changed bit suppliers and ran into a variety of different speeds. At present we are using an Onsrud tripple flute at 26M per Min and 16,000 rpm. Getting nice clean cuts and good holddown.

One problem that the supplier noticed was that the 10mm outline tool was being used to plunge TZ20 holes and the like and suggested that this would shorten the lifespan of the bit. At present we are changing the settings to dedicate one 10mm for outline and another for plunging.
We also have two bits set aside, one for MDF the other particleboard.

I have asked questions about this on a variety of boards and forums and find that it's not uncommon to get 300+ sheets per bit. Another factor that has been mentioned to get this kind of life has been the quality of the board.

Thom Davies · Post by **Thom Davies** » Tue, Sep 06 2005, 6:08PM

Hey Glen hows it going?

Just wondering what onsrud cutter model number you are using as we have just brought 2 60-126MW cutters. what speeds and cutters do you use on mdf?

Thanks

Thom Davies.

Glenn Van Reason · Post by **Glenn Van Reason** » Tue, Sep 06 2005, 6:15PM

Hi Thom,

Same one as we have the 60-126MW, nice tools.

On MDF I just turn the speed down to 70-75% seems to work well, I did notice that yesterday the guy using the machine left it at 100% but I can't be sure he cut the MDF with it.

So our standard speed is 26M per min and 16,000RPM for particleboard
and that'd make it between 18 - 19.5M per min for MDF at 16,000RPM

I checked the bit out this morning and it looks really good, no discoloration or residue at all.

I'll update on how many boards we get from this bit.

Nick M Singer · Post by **Nick M Singer** » Wed, Sep 07 2005, 12:27AM

Morning all! Seem to be getting some contradictory ideas here! Iam particulary interested in those postings mentioning a 26M per Min feed speed. Wow! that is flying. I will give it a try and let you know. As far as the diamond cutter is concerned the one I have is an \"up down\" but the cutting edges are chipped to hell after very few boards. I was told this was due to heat.
Thanks

Glenn Van Reason · Post by **Glenn Van Reason** » Wed, Sep 07 2005, 12:57AM

Please let me stress one point, this cutter is a tripple flute with upshear, at this speed we have to monitor vacumn hold down closer than we normally do, any degredation in spoilboard leading to loss of suction means smaller parts WILL MOVE!!!!

BUT when taken into account even recutting the odd part that moves it still is fast machining, the heat generated in the bit is also a lot less..

Also we have not fully tested this, so far the life is pretty good, we are at 20 sheets of chipboard and 13 sheets of MDF ( we decided to test the bit on both and see what happens) from this bit with no visiblc chipping.

Got a big nest tomorow that should test it as we come up to the 40-50 odd sheet mark. I'll post an update as soon as we get some sheets out.

Bill Rutherford · Post by **Bill Rutherford** » Wed, Sep 07 2005, 4:56AM

Glenn,
Just curious, are you cutting particle board and MDF with that bit or Melamine over particle board and MDF. If you are cutting melamine then when you run your hand down the corner where the face and edge meet as you get up near 30-40 sheets how does that corner feel? Is it smooth or slightly jagged? Also on average what size parts are you cutting? We are using the Onsrud 60-123MW at 400 IPM and 18000 RPM, on average we get 15-20 sheets of mid-size parts before we start to loose edge quality or start to get a chip at the break through point of the ramp. We are cutting melamine of partcile board. Also are you sharpening or replacing? Thanks.

Bill R

Post by **Jason Susnjara** » Wed, Sep 07 2005, 7:51AM

Guys,

Another consideration would be the cut direction. I seem to find that a conventional cut will give me a better edge than a climb cut. At one point I used the 3/8 tool for the outline but then switched to a Vortex .5 3 flute compression bit. I love this tool. I run at 18000 rpms and around 700 to 800 inches/min. But I do not cut in production runs either. The laminate will play a role in this as well. I can cut all day long here using the melamine that we purchase and the Vortex 3/8 compression tool, but when I went to the Woodmex show in England, that same tool didn't even last through one sheet. There was a tooling company that helped us out a lot at the show letting us try different tools from diamond to other solid carbide tools. We found a few that worked pretty good. A .5 diamond tool that worked and believe it or not the vortex 3 flute .5 tool worked just as good. I had to slow the feed speed down for the diamond tool just because it didn't sound that good when cutting at high speeds.

Bill Rutherford · Post by **Bill Rutherford** » Wed, Sep 07 2005, 8:42AM

Jason,
Do you know who's melamine you are using at Thermwood? You are correct that the melamine has a lot to do wih it. I find we get considerably better results from Panval melamines then we do with with Tafisa melamine.

Bill

Post by **Jason Susnjara** » Wed, Sep 07 2005, 9:09AM

Hi Bill,

We use Duramine Thermofused melamine.

Nick M Singer · Post by **Nick M Singer** » Wed, Sep 07 2005, 9:40AM

Howzit guys!

Just tried a 2 flute 10mm compression cutter at 16m a min @ 18000 RPM seems to love it. I tried my second Lach Conomic diamond 1/2\" tool at 10m per Min @ 18000 RPM and that started chipping right away although the tool edge looks good.

Glenn Van Reason · Post by **Glenn Van Reason** » Wed, Sep 07 2005, 3:55PM

Hi Bill,
We are cuttig melamine over particleboard and and colour laminated MDF. The rough edges is what we are trying to get rid of, we have only been able to get 30 odd sheets before chipping occurs. This tool is holding up a bit better but I will wait till we get a few more sheets through on it to make a definate descision.

Part size is everything from 2400x1200 pantry backs to 40mm fillers. Sorry for the metric it's too early for conversions at the moment here lol

We have tried sharpening and managed a whopping 3 sheets from our last tool that was done heheheh so we replace. I was told by one of the tooling companies that we should only expect half the sheet run from a new tool.

I have to agree with Jason that the melamine supplier is a big part. One thing we did was the last tool supplier that came and was showing us their range (the onsrud) we said ok do you have a tool on you? if so come out here we will put it in and run a few sheets and you can let us know right away what we are doing wrong/right.

This was great as they gave us a few tips and was seeing the tool in action on material and parts we actually cut. Much better than trying to imitate the chirping sound of a bit over the phone to a rep lol !!

PS we are up to our third melamine supplier at present ( gotta hunt for the best price! ) so it's hard in our situation to get a good comparison.

Thom Davies · Post by **Thom Davies** » Wed, Sep 07 2005, 4:39PM

Hey Glen how's it going?

Where are you in the world? Just wonding cos u r using metric not inperial!

Cheers
Thom Davies