PDA

View Full Version : series1 cnc 1"rougher?



sdeering
12-13-2011, 10:51 PM
Hey all.
I have a Bridgeport series 1 CNC Old Boss 5 coversion.

I have a project that involves finishing a 2.5" hole 1.5" deep in 1020 steel I think.
The holes are pre plasma cut and I have to clean up about 1/8"+- of material.

I am doing this for a bud that owns a shop. He was thinking on doing the full 1.5 depth. It turns out my steppers will not hold the full cut.No big crashes but the endmill will move the whole table (losing steps).
If I cut 1/3 or.5" depth Im OK.

Bridgeport series1 cnc original steppers on 70v DC. Steppers wired in series and Mach3.
1" roughing end mill 5 flute 200ish rpm and 2ipm and about a 1/2 dia leadin/out, water oil flood coolant is what I had it programed at.

Would wiring it in parrelel be of any benifit or am I pushing the old girl too hard at 1.5 depth?



Thanks for any help.

Stephen

Toolguy
12-14-2011, 05:01 PM
You're pushing too hard. Just run at .5 depth. Do a 2 or 3 thou. per side finish cut full depth to smooth out any steps.

macona
12-15-2011, 02:00 AM
And no real reason to run a cutter that big. I rarely use one over 1/2". Try a carbide rougher from Lake Shore Carbide. You will move more metal way faster than what you are doing now and less strain on the machine. You can either take big bites and move slow or small bites and move fast. The latter is what most people do nowadays.

sdeering
12-15-2011, 11:13 AM
Thanks for the help fellas.
Never really stress tested out the mill yet. I mostly do light work with it till now.

The .5DOC at 1/8 seem to be working. No steps lost and no real step from one pass to the other. The hole tolerance isnt too tight.
I have about 50 of these to do so Im looking for ways to speed things up a little. But if it is what it is, I will live with it.

I read my programing manual and it says 1.5 cubic inches per min. 3/4 max drill size. Pretty vague.
I did the math and I have about 3 cubes to remove. So if im understanding this correctly if I have a circumference of 4.9ish.inches and 3cubes to remove. It sould work out to 2.45 min wich is pretty close to normal feed rate of 2"/min. Mind you The 1.5 cube"/min may have nothing to do with stepper torque or tool side loading tool sharpness. I dont know Im just a hobby machinist.

My bud that runs a machine shop is contracting these out to me. He purchased the 1"roughers and holder. He is worried about getting under the plasma area to extend the tool life.
With a 1/2" carbide rougher what DOC IPM RPM would one run? 2.570 finish hole size 1.5 deep with about 1/8 of material to remove?

Thanks
Stephen

macona
12-15-2011, 12:55 PM
Ignore the removal rates for your mill. They mean absolutely nothing. It is not relevant to how you figure speeds and feeds.

With the one I am specing:

http://www.lakeshorecarbide.com/12variableflutecarbideroughingendmill.aspx

You are looking at 3056RPM at 27 in/min feed figuring 400SFM cutter speed which is in the middle range. At 3krpm you could drop the feed down to 20ipm if your machine cant keep up.

sdeering
12-15-2011, 01:18 PM
Sounds alot faster than I am at now.
I may have to try that.

Thanks Stephen

Uncle O
12-15-2011, 06:03 PM
It appears that is only 1" LOC and the OP has a full 1.5" depth....
I have had trouble getting 1/2" carbide endmills with that much engagement
to not sing at those speeds and feeds .... Usually I have to slow it down, but would still be running way faster then the OP's speeds and feeds.

macona
12-15-2011, 07:34 PM
I have no problems running that deep as long as I do the finish pass before dropping down. Then there is no rubbing. You can also neck the top of the mill to provide the clearance. Lake Shore also sell longer flute end mills.

sdeering
12-15-2011, 10:47 PM
So you are using a .5 DOC ?

macona
12-16-2011, 11:32 AM
That should not be a problem. You could probably go 1x if you are just cleaning up a hole.

Steve Seebold
12-29-2011, 10:12 AM
Can you cut a helix on your machine? If you can, make your program so the machine thinks it's cutting a thread for the ruff pass leacine about .010 on the wall, then put in a good finisher and circle in to and out of your finish cut.

sdeering
12-29-2011, 11:20 AM
Thanks for the input.

I think with a .01" cut you would be in the leftover slag from the plasma cut alot. The cutter probly would take a beating. NO?

The .5" doc down to size 1/8 to 1/4 woc seemed to work good. This puts the cutter well under the slag (conventional milling). Slow mind you. 200rpm and 2"/min.

If the job shows up again I will probly try a carbide 1/2 rougher at faster speeds. Maybe nest time they will be pre lazer cut that would help.

Stephen