Router Tool Life

Could be between .5 sec. and 3 years. What is the material of the cutter, HHS or carbide, if carbide what is the grade? What chip load will you be running? (That is how much will each tooth of the cutter be cutting on each pass?)

Mostly you need to figure out your speeds (spindle) and feeds (travel rate) to determing cutter load. Depth of cut will make a difference in the tool life as well.

Please get back to us with:

Feedrate

Spindle RPM

Cutter diameter

Cutter material.

We are here to help.

Efim,

Back in the 1990's, I was managing the CNC shop. We had the Avenger Class Minesweepers contract and we routered All of the non ferous metals except for Stainless.

Various grades of Alum., Copper/Nickel, Silicon/Bronze, even FRP.

We were operating (2) shoda NC-163 and NC 263 Routers.

Expected tool life, depends on the bit. We used a single spiral downcut, running 7,000-12,000 RPM, closer to 7,000 barely enough to keep the inverters from tripping.
for 12 MM, we were using 1/2" dia. can get away with 3/8", the thinner material the smaller the bit.

And its been awhile, I believe about 30-50 in/min. I would have to look in to that.

One thing, because we held it down with Vacuum, we had MDF for the vacuum table,

We did not use coolant (to keep the tables from absorbing the coolant and to keep the accuracy on the table), instead we used the chipload to carry away the heat.

Some of these bits would only last less then a 100" of cut (problaly from a poor tool set) a good toolset one the could last through 2 nest sheets. aleast 2,000 inches or more.

One more thing, the harder alum. machines better than the softer. hope this helps.

This should start you out. You'll have to do some trial and error to begin with.

I do have contacts if you need them for more up to date info, you can email my.

Good luck,

phoenix911

What kind of profile are you talking about? Typically a more involved/complex geometry will reduce life.

being a production shop or any type of shop, you have to expect both.

being a production shop or any type of shop, you have to expect both.

uhh, yeah. I guess that makes sense to someone.

Thanks to everybody. Special thanks to phoenix911.

We intend to use carbide tools 6 - 10 mm with chipload about 0.1-0.3 mm @ 18000 rpm. Example of one of our parts is shown.

I had looked at my notes, which was storage, and so far when I gave you the RPM of 7,000-12,000 that was for FRP. 18,000 is correct for Alum. I am going to see if I happen to have some older programs or macros to see verify what the travel speed to use as a base reference, then the operator can fine tune it as its cutting.

Also, even though at times we were able to cut 1/2" thick in one pass, we had always took 1/4" pass cuts at a time, just due to the fact of our fastening techniques.

do not know what your tolerances are, but what I remember is some of the tooling bit even though they were the same types but from other manufacturers, we could get chatter through them. At the time we preferred Onsrud, but this was over 15 years ago. Things changed since then.

Also, hopeful your router is built heavy, because this can put quite a bit of lateral stress to your heads. I think we had BT40s and BT50s for head, Damn, I can't remember I'll have to look into this.

Also I like to add, whatever type of head you have on your router make damn sure that your surfaces on your tools are clean, if it isn't it's going to fret due to the high frequency vibrations. And changing from one tool holder to another or to different heads, it will spread.

Sorry, one more thing... we had better luck???? with high speed steel bits, these hold up to the high speed vibrations better with no coolant. Didn't take us long that this made sense.

And if your operating with the chip load to remove your heat, wear closed gloves.

because of you, these things that were once lost, are coming back little bits of memory at a time

Which bring one more thing, depending if you can fasten it, if the part is too small and it moves while your cutting, there are some things you can do. This is IMPORTANT.

1.) fasten (screw) the stock to your table.

2.) If you have problems holding vacuum, leave in tabs on the cut between your part and stock material, so your part does not fly out or leave approx. 0.003-0.005 of material left, it's only be foil but your on smaller puts it works great.

I am saying this because we had I lot of development on cutting wood, metals, composites and such that our shop was a showplace for Shoda to show the versatility of the routers. (we had quite a bit of international tours there.) and was a good selling point for Shoda.

again best of luck,

phoenix911

Thank you very much for your kind and valuable instructions, it is very useful to our customers also to us cutting tools manufacturers. You are right phoenix, we should be more careful with relatively slow speed, especially while engraving and cutting hard materials, to make good use of the tools for our machining work.

Dear Mr. phoenix, I am very happy to meet you here, hope we could be good friends in the near future, and I hope we could have the big honor to let you test our ASTECH Tools Life. We believe you will have new discoveries for the cutting tools life for CNC Route machine. Hehe

Hope all best with you there!

Best wishes from friend Alice

Dear friends,

Estimating cost of machining (Al 6061T6 8 mm), I take feed rate 1.7 m/min and tool life 50 m. At price of tool about $100 per piece, the main part of cost is due to tool ($2 per meter of cutting). Am I right?

Hello Efim

sounds about right, good follow up.

It was rather costly for us to0, but for us there was more to it.

When I was running the shop at the shipyard there were a few more variables to be taken into account as opposed to cutting the piece from other types of operations, such as plasma.

This could be that the parts have to be dipped, dimensional stablity due to heat, as well as finish. the cost analysis (did allot of that in the yard) between the operations was pretty much a wash. So it came down to the shipfitter preference which was router due to the quality.

phoenix911