[cwaugs]

Searched forums and I suppose I am the only human that doesn't know this, but my main issue right now with my YCM-40 converted to MACH-3 CNC mill is how to clamp a big piece down so that it don't move when I machine it. Have the t-slot bolts and hold downs but two of them tightened down as much as I dare still lets the piece move if I kick the speed up. There HAS to be a sticky somewhere but I have yet to find it. Thanks much, Wayne

[fizzissist]

When in doubt, always add one more clamp than you think you need. When you're done adding that one.. add one more.

Is it moving left? Then put something in its way. Is it shifting right? Make it stop. Or.....don't go so fast.

And always remember 3-2-1 locating....and clamp around that.

[cwaugs]

Going to take some getting used to. Also the mill speed how slow is too slow. Seems too fast won't allow the bit to clear itself? Had one plug up on me and couldn't figure out why it was acting so crazy and messing up the piece. thanks again. Off to milling stuff. Wayne

[fizzissist]

Going to take some getting used to. Also the mill speed how slow is too slow. Seems too fast won't allow the bit to clear itself? Had one plug up on me and couldn't figure out why it was acting so crazy and messing up the piece. thanks again. Off to milling stuff. Wayne

Ya know, posting some numbers and conditions might help us help.
Stuff like workpiece material, cutter material, dia, rpm, feed rate, coolant or not, depth of cut, engagement (relative to dia of tool)....and stuff like that.

Sometimes simple answers will help simple problems....if we know simple parameters.

[cwaugs]

I know, I'm too new at the supermax to even know the numbers. I cut a 3.93 in hole in a 1.5" thick piece of aluminum with a .750 2 flute and was used to a Cnc router running at 10k rpm so thought the big machine should run screaming too. Seems that slowing it down to probably roughly the same speed that one would use to drill with , or maybe a bit faster, helped a lot. The rpm on the machine is irrelevant as the VFD as well as the variable speed and the two speed on the head make it a guessing game as to the speed. Need to get my hand held tach out and see if I can center it on the bit to get an idea what I'm twisting it. As far as the speeds I end up cutting approximately .200 at a clip and the speed in Mach3 I run down to about 4-6 would it be IPM to keep from moving the piece due to my lack of clamping ability. This machine is such a change from my small router in that it is capable of going as fast as I want as well as wherever without asking any questions. I'm definitely leaning towards the caution side until I get the hang of it. How fast can I take a .750 2 flute through a piece of Al. .5 deep full cutting width? And why does a 4 flute the same diameter plug up so easy with aluminum. Seems my router didn't do well with 4 flute either. Thanks again for the invaluable help. Wayne

[fizzissist]

1000rpm at 6ipm feed with a 2fl HSS 3/4" endmill should be a VERY comfortable starting place that won't get you into trouble. You are getting a good air blast or coolant flow into the cutting zone, right? Clearing the chips out is probably your biggest problem with the 4-flute. Otherwise, they work just fine.

Don't go more than 1/2 the dia of the tool in a full width cut at a time for starters, and plan on making a finish pass, climb cutting, maybe .020 finish allowance with the full length for clean up, because you'll have over-cut ridges on the part where the bottom of the tool was that are deeper than the upper parts for each pass.

If you get chatter? Slow the RPM, first, then increase the IPM...till it quits. Chatter is nothing more than resonance.

For ramping into the part in Z, you can feed the tool down into the part very nicely at no more than 3 degrees relative to the surface of the part. That will let you eliminate a pre-drilled hole operation. On a CNC it's a piece of cake.

A .200 step-over should be no problem for a 3/4 endmill at all. And Btw, get a grease pencil, calibrate your spindle speeds, and mark the numbers on the handle so you know where you're at.

[cwaugs]

You lost me on this part. Are you talking if I were to be cutting an angle piece?
<For ramping into the part in Z, you can feed the tool down into the part very nicely at no more than 3 degrees relative to the surface of the part. That will let you eliminate a pre-drilled hole operation. On a CNC it's a piece of cake.> Again, excellent info and thanks much for your time. Wayne

[rowbare]

Workholding is almost a field of study in itself. There are several books published on the subject. It helps a lot to understand certain basic principles.

Chapter 2 of this book: Setup reduction through effective Workholding explains things nicely and is available in the Google Books preview.

bob

[fizzissist]

You lost me on this part. Are you talking if I were to be cutting an angle piece?
<For ramping into the part in Z, you can feed the tool down into the part very nicely at no more than 3 degrees relative to the surface of the part. That will let you eliminate a pre-drilled hole operation. On a CNC it's a piece of cake.> Again, excellent info and thanks much for your time. Wayne

Think of a flat piece of material, its surface is a Z0 for your program. Z+ is above the part, Z- is into the part.

Let's put your tool at Z0 (just kissing the top of the part) and X0,Y0 (in this case right in the middle of the part).

If you program:
G0 X0 Y0 (LOCATE TOOL OVER START POINT
G0 Z.1 (BRING TOOL DOWN IN RAPID
G1 Z0 F3. (FEED TOOL TO TOP OF THE PART SLOWLY FOR SAFETY
G1 X4. Z-.21 F6. (RAMP DOWN INTO PART AT 3 DEGREE ANGLE
G1...or G2, G3...whatever. You're into the part now

You've moved the tool over 4., down .21... or 3 degrees

Any good CAD/CAM program should offer a ramping option, either in a straight line or a circle (which is ideal for milling out holes or pockets) and give you the options for step over, lead in/lead out, modifying feed rates, etc.

[Shane1234]

use dowel pins sized as the same width as your t-slots to stop it from moving in your Y direction. as for the x direction, i like to use 1-2-3 blocks bolted down, or a simple square bar with holes for across the slots. that will stop your part from sliding. you will still need to clamp the part down. we feed our supermax at 45ipm thru stainless(by holding the rapid button down), .2 depth of cut, 800 rpm, 2 inch wide 45 degree facemill. not one issue.