Help milling exhaust flange

[pauls]

I have a IH cnc mill. I've been milling exhaust flanges for turbo setups. These are out of 1/2" mild steel. My process is very time consuming. First hold steel to pre-tapped aluminum plate and drill bolt holes and lead in holes for the exhaust ports. Bolt the drilled plate to the aluminum plate and machine the profile in 1/16" increments. This seems very slow and tough on end mills. I'm no machinist only a hobbiest. How would a professional approach this job?

[Runner4404spd]

waterjet or laser depending on quantity and quality required. for one offs a mill is not that bad. also make sure your using carbide tooling. i have also upgraded to a 3hp motor. how large of an endmill are you using?

[Geof]

The way you describe sounds pretty standard and probably the biggest difference between your procedure and that of a 'professional' would be the increment size.

You do not give any speeds, feeds or cutter information but depending on the shape of the profile and any concave curves that would limit the maximum cutter dia. I would start with a 3/8" or 1/2" four flute cutter running at around 400fpm, i.e 4000 rpm for 3/8" dia. or 3000 rpm for 1/2", a depth of cut around 0.2", an increment of around 0.2" to 0.3" and a feed of 0.002" tooth which would be 32 or 24 ipm with a good strong air blast to clear chips and cool the cutter.

Probably you do not have anywhere near enough power and maybe not enough machine rigidity to do this.

You could consider doing a bit of experimenting if you have not done so already. There is naturally a relationship between all the parameters I mention above and the power needed. If you increase the speed you need to decrease the depth of cut or increment or feed, and vice versa. It is possible if you dropped your speed to something that seems unreasonably slow when expressed in feet per minute you might gain enough extra torque at the tool to increase your increment or depth of cut to more than compensate for having to run the feed slower to keep the same cut per tooth.

[davereagan]

Private message me. I make these for profit. What kind of machine are you using? I take the cut in two swipes with a 3/8" endmill, but this is not a standard 30 degree helix endmill. http://cgi.ebay.com/ebaymotors/ws/eB...185300053&rd=1

[pauls]

Thanks, I'm using a 1/2" four flute cutter carbide but as you mentioned the machine is not rigid enough to do more than about 10ipm and max. speed is 1800 rpms. I'll play around some but at least I'm on the right track.
I have a cnc plasma cutter and with 1/2" material I can't achieve the accuracy I need.
Paul

[davereagan]

Paul,
Many people are not aware of the new variable helix TiALN coated carbide endmills and what they can do when run right. First of all, you get longer tool life dry than wet. 400 sfm with high engagement is normal for mild steel. 500-600 sfm is fine for finishing. To cut your piece, I would use a 3/8" Garr VRX endmill at 4000 rpm and .002" feed per tooth. 4 flutes, so that's 32 inches per minute. I would take a 1/4" deep cut full slotting and on the second pass, I'd go .800" deep so the wear is taken higher on the flutes for the second cut. The price for this endmill is ~$25.00 or $44 for a 1/2" but the productivity is well worth the cost. I used to cut 3/8" flanges in one pass and then a clean up pass with a 3/8" endmill. I once ran 80 pairs of the flanges I have listed on one endmill. This is using a 40 taper machinig center with box ways. With your smaller mill, you may need to take three passes, but this is still far faster than your current program. You can find these endmills are www.reidtool.com Email with any questions.

Dave