Question on chipload / bit selection

[lrheimpel]

I am cutting 3/4" OSB sheets using an Amana 46178 3/8" 2 flute Solid Carbide Compression bit. I am cutting at 21,000 RPM and 5 in/s or 300 IPM. This is industrial production so cutting faster would be helpful.

Found Amana (http://www.toolstoday.com/p-6265-solid-carbide-compression-spiral-bits-for-cnc-nesting-operation.aspx?&variantids=11845,0&keywords=46371 ) has a 3 flute bit that according to the graphic can do a 1xD pass at close to 800 IPM or 13 in/s @ 24,000 RPM.

Using Shopbot's chip load calculator I get this bit is capable of doing a chip load of 0.011 in/flute. Using same calculator solving for speed at my router's speed (21,000RPM) I should be able to run this bit at 11.6 in/s or 696 IPM.

In other words, using the Amana 46371 bit I can do the same cut at twice+ the speed of the Amana 46178 bit.

Is this correct? I am not experienced in doing these calculations.

[jerry_stanek]

I would keep bumping the speed up and listen to how it sounds. You should hear where it cuts the best by the sound.

[Kyle Stapleton]

It would be helpful to know what bot you are running.
From my understanding the fastest the alphas can cut are 10ips, that said if you can drop you RPM's you can run a slow feed and still get the right chipload.

[gundog]

Here are some formulas you can play with. The bit maybe capable but your machine may not be that is a pretty agresive chip load.

FORMULAS: Chip Load = Feed Rate / (RPM x # of cutting edges)
Feed Rate = RPM x # of cutting edges x chip load
Speed (RPM) = Feed Rate / (# of cutting edges x chip load)

[garyb]

Any major tool manufacturer will test all tools going into production and work up and set a recommended chipload to suit the grind of the tool.
I cannot say for other manufacturers but for Onsrud you will find the chipload of each tool series and for type of material being cut in the back of the catalog. (available as electronic or hard copy)
You can then use the formulas gundog has noted above as a starting point to fine tune feed/speed for the given chipload to suit your machine.
therefore you should contact your tool supplier/manufacturer for the recommended chipload of your selected tool, this is the recommendation to get the maximum life out of your tooling, of course you can also just wing it !
Gary

[Ger21]

I've never cut OSB, but my guess that you'd want around double the feedrate and about 18,000 rpm.
If your machine can't handle that, back off both feedrate and rpm proportionally from there.

[garyb]

I just looked up the standard for 3/8 compression 3 flute for osb. recommend chipload is .020 so at 3 x D would figure to 630ipm at 21,000
so your real close
Gary

[bleeth]

He better have a well tightened Alpha with a 4HP min spindle and very good holdown to run that speed.
I have found best cutting speed to be around 6ips (360ipm) on my Alpha, but am usually using smaller bits.
I also see our original poster hasn't replied back yet to any comments made.

[garyb]

Then again Dave, he might not have a SB :eek:
Gary

[bleeth]

Just checked his previous posts.
I think he has a Buddy with a router. Don't know Standard or Alpha.