2D DYNAMIC AREA FEEDS/SPEEDS

[FTI2007]

I wanna try using a dynamic area mill to do a pocket and I have had limited success in the past. material is A36. I will be using a standard garr 4 flute carbide 1.5" loc cutting 1.125 deep. I wanna do it in 1 depth cut. What is a good safe starting spot for feeds and speeds. I looked at the database but that seems to be mostly special coated endmills. any help is appreciated. Thanks

[cunder]

I would use what Garr recommends and the use a calculator to adjust for chip thinning.

Dapra has some for different tool and You can download Yourself.

 

http://dapra.com/tech/calculators.htm

[jeff]

I will be using a standard garr 4 flute carbide 1.5" loc cutting 1.125 deep. I wanna do it in 1 depth cut.

Definitely look into getting a variable helix endmill.

 

Also "1.5" loc cutting 1.125 deep. I wanna do it in 1 depth cut"...... this makes no sense

What is your endmill diameter?

How deep are you wanting to go?

What stepover are you wanting to use?

[djstedman]

You don't mention the diameter of your cutter.. so its hard to give an answer really, I am assuming your probably using a 1/2 cutter? or possibly 3/4 .. my suggestions of SFM will apply for either however my RPM's will be based off a 1/2 inch cutter. The smallest cutter that gives you the rigidity you need will probably be better since you will get more RPM at the same SFM from a smaller cutter, more rpm is going to be more teeth in the work and more teeth is going to buy you a higher federate.

 

As for coatings they are using coated cutters because then you make a huge bump in allowable surface footage, an uncoated cutter will not hold up as long at high surface footage, that said in A36 .. Garr recommends 250 to 300 for uncoated carbide in A36 so middle of the road would be 300SFM at 2292 RPM, however in dynamic milling applications you tend to be able to get away with a bit higher SFM due to the lighter axial depths of cut.. so I would suggest pushing it to about 400SFM to start, so 3056RPM, in fact you might find your able to push this up some, I know they recommend 300-500SFM for their coated mills and I have run them at 700SFM without problems in dynamic mill applications.

 

Anyhow that said.. your chipload per tooth is going to be very dependent on your stepover, a good starting point for stepover is between 10 and 15 percent of the cutter diameter at 12.5 percent in a 1/2 cutter your looking at a stepover of .0625 using radial chip thinning calculations, that would be 18.5 IPM at .001 IPT, 40IPM at .002 IPT and 55.5IPM at .003 IPT

 

So anyhow.. if you got this far.. on a 1/2 inch uncoated cutter I would probably start at 3100RPM at 55IPM and see how it went.. definitely flood the hell out of it with coolant to flush chips.. and have fun..

[FTI2007]

Sorry for lack of info. a little distracted today. Yes 1/2" diameter. As far as the 1.5 loc is because we have 1.00" or 1.5 loc and I was hoping to do it in one cut if possible. We dont get the liberty of ordering anything we want here. small shop and they seem to stick to the cheap stuff. Just trying to make the most of what we have. the chart I have from garr says sfm of 175 -250. It just seems that when dynamic paths are considered the numbers used are no where near the recommended so that is why I was asking. I was also thinking 10-12% step over. Thanks

'

[jeff]

Is your endmill uncoated?

If so, you want about 4200 rpm, 90ipm with a 10% stepover for your 1-1/8" depth of cut

And flood the hell out of it with coolant

[crazy^millman]

Is your endmill uncoated?

If so, you want about 4200 rpm, 90ipm with a 10% stepover for your 1-1/8" depth of cut

And flood the hell out of it with coolant

 

Yeah was trying to push a 3/8 endmill yesterday to 20% step over in 7075-T6 sticking out 2.1 and it did not like it very long. When I backed it down to 10% step over it handled it very well. I think with a .75 stick out I could go up to 25% step over to do part of it and then come back with the 10% step over for the rest, but trying to ease the customer into HST and not shove it on them. They liked what they saw yesterday so look for more to come. We saw a 47% reduction using HST with a 3/8 endmill verse the traditonal method using a 5/8 endmill then coming back with a 3/8 to clean out the extra material. Engineers and their .2500R +/-.001 on a housing. Guss I should add 1.9 deep as well. :wallbash:

[djstedman]

lol crazy.. just be glad its not .062 +/- .001 on an internal corner.. 2 inches deep .. I hate when they pull that crap.. but they all seem to do it..

[crazy^millman]

lol crazy.. just be glad its not .062 +/- .001 on an internal corner.. 2 inches deep .. I hate when they pull that crap.. but they all seem to do it..

 

Oh I got some them floating around right now and love the sharp corner on a part where I need to take 15 deg sharp point tool and make it happen.

[Jeremy Herron@DBS Solutions™]

Lol. My favorite response to these types... Just because you can draw it doesn't mean you can make it. Now ask me again why your part is so expensive...

[Chris Rizzo]

I've run lots of dynamic paths with all sorts of tools; from 250$ Sandvik Plura's to 50$ Garr's. Quality tools you can run over 500ipm at at 800sfm. Value-priced tools you can't get that performance, but can still run circles around traditional large tools / slow feedrate toolpaths. (IMCO power-feeds aren't much more than garr's these days and run very well).

 

A few things to think about-

 

You could very well make way more money with a high-performace tool. Provided you have a good production part, and a good machine and holder that can run it. You gotta run some numbers and some testing to eek the performance out, but a 5x more expensive tool could make a part 10x cheaper through cycle time and machine utilization alone. Thats IF you run the machine fast enough to use the tool.

 

Ok back to your question.. with a regular 4 flute garr, 1" doc, 10% stepover. 3500rpm (430 sfm). 100 ipm to start with, increase feed as fast as your machine/holder/part will take. It's not the feed that is going to kill the tool. Don't be afraid to turn it way up. I wouldn't be suprised at all if 150 ipm works. Cheaper cutters don't seem to have good core-thickness/grind, so you will see some flex. Since you don't have a coating, keeping the stepover low will keep the heat at the cut down. Coated tool you could handle more heat at the cut and probably increase stepover. No coolant. Heat will be in chips and not part. Air blast works well.

 

For a little at-the-machine tuning, watch the chips very closely as they come off the cut. Should start silver, and then by the time they land should be blue/tan. If they are blue too soon, your rpm is too high. If they stay silver, turn up the rpm a bit. Whatever you come up with for rpm, feedrate is always as fast as your setup will take. It's speed not feed that kills.

 

If you need a finished floor: leave .025, and copy the toolpath. Then set stepover to 40% and leave 0.

 

Let us know how she runs.

[FTI2007]

Thanks everyone for any input you gave. I ended up doing it the old fashioned way last week because I didnt have the time to play around as the management decided they couldnt wait. But Im going to print off this forum for my notes for the next chance I get to do somthing similar. Chris where or how did you come up with a starting point of 3500rpms and 100ipm And just FYI this is going in a 40 taper hass if I already didnt mention it. Thanks again.

[Chris Rizzo]

In all honesty, the seat of my pants and doing it a lot. I've followed manufactures feed & speed calculators to the tee, even the fancy Sandvik calculators that are stand-alone programs, and invariably find running beyond their high end numbers with no diminished tool life . Sometimes well beyond their numbers. Tougher/harder more specialized materials I will be close to their numbers, but above A36, 1018, 1045, even A2, etc and every flavor of aluminum. (Aluminum has no surface footage limitation). I attribute it to the low radial stepover. With a 10% stepover, 90% of the tool is out of the cut and cooling. The heat generated in the tool is nowhere near a traditional 40-100% stepover, which is where a lot of the sfm calculators come from.

 

So yes it may be a bit shade-tree sounding...But doing, hearing, seeing, smelling, and feeling go a long way.

 

I get a fair amount of demo tools and occasional can't even break them when trying. AS long as it's programmed correctly to not mechanically overload the tool. (stepover, entry, rounding rad, etc)