How Should I Machine This?

[Metal]

Just a quick question really
apparently image didn't post, here
https://s10.postimg.org/hy9c8gjp5/dive.jpg



I'm still figuring out the new CNC, I've noticed that when coming around a corner, the bit has a tendency of being pulled up into the work exactly how I assume it would be due to the forces on the bit (note this is all roughing passes)

I "assume" this is unavoidable with a machine that has backlash since the mill moves upwards, then the torque from the cutter is what is dragging the table across the backlash zone and into the work before the cnc compensates. if I was doing this manually I'd lock the table, which the cnc can't do.

So my questions are
1: is this avoidable (I'm guessing not)
2: again assuming not, how much stock should I leave around the part for a finishing pass, My assumption again is around 2x the depth of the "dive" or .05", which ever is more, since passes less than .05" in aluminium tend to not cut it very well.

 

[dlane]

I'll guess you are useing tapatalk camera icon , not paper clip , all I see is the infamous red "X"

 

[jbolt]

What is the machine, material, cutter, depth of cut, width of cut, feed rate?

 

[JimDawson]

I fixed the picture for you!

The first thing I notice from your picture is you are conventional cutting, if your machine will do it, climb cutting is the prefered method.

The next thing I notice is that your feed speed looks a little fast for the spindle speed. Maybe bump up the spindle speed or slow down the feed. Your cutter could be a bit dull also, maybe try a different cutter. Are you keeping the tool wet with coolant, I see what looks like fuzz ''welded'' to the surface.

Maybe try taking smaller bites, both depth and step over, it takes longer to make the part, but the quality generally goes up. In the home hobby shop time is not normally an issue. If you are doing this for profit, then some maintenance on your machine might be in order. Maybe just snugging the gibs a bit would be helpful.

I normally leave 0.010 for the finish cut.

 

[Metal]

Thanks for the advice, this was purposely roughing to test the cnc's accuracy at a higher load and with an old dull cutter since I wasn't sure if it was going to snap at this speed, I was just looking to address the dive issue circled at this time.

This is with a 3/8" endmill @ 1100 or so rpm, ~14ipm .1" doc. 6061 aluminium These servos could easily exceed 100ipm so I'm being gentle, I'm trying to resolve issues as I move up to a hopeful 20ipm cutting rate rather than just start at that rate and break a bunch of things figuring it out.

I am conventionally milling because the bridgeport doesn't have ball screws and its going to be less problematic.

 

[Billh50]

Jim is quite right in what he said. If your machine is not rigid enough you may want to take several passes conventional milling and leave about .015 for a final pass climb milling. Climb milling tends to leave a much better finish with the right speed and feed. But definitely use either a spray or flood coolant to keep chips from welding themselves to side as the cutter passes.

 

[Metal]

so how would that address the dive issue illustrated above?

 

[jbolt]

Your spindle speed is too slow for a 3/8" 2-flute cutter in aluminum for that feed rate. Would be okay for a 4-flute but with aluminum they don't evacuate chips well and tend to load up even running flood coolant.

I wouldn't recommend experimenting with a dull cutter. I don't think you will learn much other than dull cutters produce poor finishes.

I suspect the over run issue is the backlash on the lead screws. Are your gibs snug?

 

[JimDawson]

so how would that address the dive issue illustrated above?

Using a dull cutter will increase the dive. The cutting pressures are much greater and much more spring in everything. The cutter is doing more rubbing than cutting, especially when conventional cutting.

Here is a staged picture of a bearing mount I machined last night just to put things in perspective. Material is 6061-T6


I still had the G code loaded so I fired up the machine and grabbed a screen capture of the running machine cutting air.

The DOC is 0.125, a sharp solid carbide 3/8 end mill, climb cutting. Kerosene in the fogless coolant system. Finishing passes were at 0.010

This is real time cutting parameters. The inputs come from the G code, actual spindle speed, and actual axis vector speed. The cutting speed and chip load are calculated from the inputs. Also accepts manual inputs for calculating feeds and speeds when not running.



This may help a bit getting you started in the right direction to address the issues.
.
.

 

[Boswell]

I'm not sure I understand your initial post. Are you implying that you have 0.05 backlash? If that is the case, you probably need to figure that out before making parts. No amount of optimizing feeds and speeds or coolant will fix a 0.05" backlash. I also tend to leave 0.015" for a finnish pass and use climb milling most of the time. For a 0.375 two flute cutter. 0.1 DOC at 1100RPM and full cutter width slotting, GWizard sayd that a very aggressive rough cut would be 7.9 IPM and (as a hobbyist with more time than money) I never use the most aggressive end and for roughing using go about midway between aggressive and conservative, in this case GWizard recommends 4.8 IPM . I typically cut using 2750 RPM and in this case that would allow the 4.8ipm to increase to 12.3 ipm. Also note that GWizard assumes you have proper chip removal in place (Flood coolant, or Misting system etc).