[bassdo]

I have a part that the width (Y-Axis) is .750" and I am putting a slot through it that is .755" wide and depth of .750". Material is 304SS and I am taking a .02" cut per pass with a carbide 1/2" 4FL end mill. The first operation is 5 hours and 36mins. I have two more operations which is even longer. I need to drastically speed this up. What feeds and speeds should I run. Currently running at 918rpm 1.8 feed. I have a HAAS VM 2 and max rpm is 12,000. This is our first time having high speed machining and we just are not sure about feeds and speeds to run. I can not get it to program the tool path I want. It just runs straight back and forth through the part instead of doing the high speed circles pecking at the part. I will post a picture to show you what tool path it is producing.

[Bm150]

Mainly depends on the tool you are using. I would use a high speed slotting cycle witch will take a deep cut but only engage with small amount of cutter at anyone time. This will save the tool too. As cutting it all with the same 0.02 won't last long.

Up load file and someone would love to help.

All the best

Sent from my HTC One using Tapatalk

[rowbare]

I think you need to spend a bit of quality time with a good feed/speed calculator like GWizard or FSWizard. You aren't doing yourself any favours trying to baby the cutter with a .02 depth of cut. .25 or would be more like it.

Given the width of your slot, why not a .750 cutter, ram straight through it say .700 deep then do a couple of clean up passes at full depth to get to your final dimension. That should take less than 2 minutes.

bob

[tony978]

My two cents is cut .005" above depth and peal mill that . But that is me and I hate milling 304


Tony

Sent from my iPhone using Tapatalk

[fizzissist]

?????
Get yourself a good 2 or 3 flute insert mill, with the right inserts. You can get them as small as .5" .....
With a 5/8" 2 flute, you can easily run it at 4500rpm and 36IPM feed. DOC will probably work out to .120 + for roughing.. depending on
the insert specs. Bolt it down, run it dry, let it fly!

I don't know why people are so freaked about 304SS. It's not that tough, more on the gummy side, but it will work harden so you can't dwell
or baby it.

At .02" DOC, you're just wearin' out your cutter. Even with a solid carbide at 325SFM you should be in the neighborhood of 2000rpm and 20IPM.

5 hours? The time saved getting the right tool and running it the way it was designed will more than pay for itself. I'd be pissed if that operation took 20 minutes,
rough and finish.

[tony978]

Ya just don't try a Mitsubishi apx and run it with specs from the book . I showed there rep how quickly I could make a paper weight !


Tony

Sent from my iPhone using Tapatalk

[cadcam]

I would follow Tony and I have NO issues cutting 304SS. use the slot mill you can use the 1/2 tool you said it is Carbide 4flt is it coated ? Who makes it.We should get this to 15min less cut rough and finish,
You said it was basically 3/4 x 3/4 x 3/4 correct?

[LeeWay]

I too would cut deep and come in from the side. The flutes on the tool will last much longer than the teeth.

[bassdo]

Thanks for all the feed back. We are new to high speed machining and trying to figure it out. It is roughly .75 X .75 X .75 I ran it with a 1/2 EM non coated. No matter what I did I could not get it to give me a tool path where it plunged outside of the part and than ran through it. I didn't have time to mess with it, being that we needed these parts finished asap. I will get some scrap 304 SS and try the methods suggested.

[LeeWay]

I do not have Master Cam, so cannot comment on that exact procedure, however a work around would be to just draw up a series of lines that you want the end mill to follow. Stay just shy of the finished depth and width. Then at the end, do a full depth and width pocket finish pass.

[tony978]

hope this helps got to love youtube !
http://youtu.be/TlYg3J8riIA

[cadcam]

Always good videos from Mike.

[LeeWay]

Nice! I can see why people rave over Mastercam. Looks very well equipped with a nice UI.

[bassdo]

I have a 16.125" long by 3" wide 304 SS I have to basically make a pocket in. I have to remove a lot of material. 1/2" Carbide TiAlN coated. Does running 2483rpm at a federate of 20.0 at DOC of .5" sound reasonable? It is a 2D high speed area tool path. Whenever we try to do full DOC in 304 we break end mills.

[tony978]

I am not sure is square corner will last depending how your holding the part , I know if it can vibrate there goes your cutter !!! Most of the 304 I have run is not ridge when done or to start with so I have a strong dislike for the stuff


Tony

Sent from my iPhone using Tapatalk

[bassdo]

I just ran a practice part. 304, DOC .5" and .02 stepover on a 2D high speed area mill tool path with 1/2" square end mill 4 flute non coated at 10000rpm and 100ipm. Ran good but tore up my end mill. Was only a 4x2" pocket. Took ten minutes but the end mill is no good now. I have some TiAlN coated end mills but didn't want to ruin those trying super fast milling.

[tony978]

Your recutting chips !!


Tony

Sent from my iPhone using Tapatalk

[bassdo]

Do you have any suggestions for feeds and speeds to run at? We are just trying to get in the ball park of speeds and feeds to run to optimize tool life and increase productivity.

[tony978]

Got to the manufactures website of the tools you are using and they will give you an idea . I would say keep the chip per tooth and drop the sfm to 150-200 to start


Tony

Sent from my iPhone using Tapatalk

[bassdo]

I have tried everything and the end mill is vibrating really bad. Tried different machining calculators including FSWizard.