Cutting inlay pockets

[Bill the Cat]

I've been doing some more playing with my CNC and thought I'd as for opinions. I've programmed to cut pockets for inlays in both clockwise (conventional milling) and counter-clockwise (climb milling). Visually, I can't see any difference in the quality of the cut.

The other issue that I have not tested yet involves cutting a detailed pocket where a larger cutter is used to "hog out" the center of the pocket and a smaller cutter is used to finish the edges of the pocket. I was curious how most accomplish this task. Cutting the center out first with the large cutter and then skim cutting the edges with the small cutter or using the smaller cutter first and the larger cutter afterwards to clean up the center of the pocket. It would seem to me that using the smaller cutter first would allow it to be in a "full" cut and avoid problems of deflection when cutting on just one side of the cutter (after the larger cutter has removed the center of the pocket).

I searched the forum, but didn't really find much.

I just don't have the time to make ALL the mistakes myself, so I'd love to hear experiences/opinions.

Let the discussion begin

 

[RBC]

Bill

You probably won't see the difference in the quality of the cut, but it can definitely make a difference in the actual size of the pocket. Go to www.precisebits.com and look at their tutorial on zero glue line inlay. It has tons of information! You should rough out with a climb cut so that any tool deflection moves to the center of the pocket and not to the outside making your pocket too big. Also, you should "profile" the pocket with your smaller bit to get your final dimension.

As for how to do two cuts, Bobcad can do this pretty easily. I have 23 and could tell you how to do it in mine, but I'm pretty sure yours is different so it won't help you anyway. Maybe someone on here with your version can help you out.

Have you tried to fit parts into your pockets yet? Depending on the runout in your spindle, you may need to adjust the cutter size you use in your g code creation. If your fit is loose, you can use a bigger number. Smaller if your part is too big.

Happy cutting!

 

[Bill the Cat]

Another senior moment

Thanks Royce!

I read the Precise Bits tutorial last year (before I actually got my CNC) and totally forgot about it. Thanks for the reminder!

I can program the cuts in BobCAD V19 with no problems. Just needed to know the best way to do the actual cutting.

 

[WilleeCue]

I've been doing some more playing with my CNC and thought I'd as for opinions. I've programmed to cut pockets for inlays in both clockwise (conventional milling) and counter-clockwise (climb milling). Visually, I can't see any difference in the quality of the cut.
Let the discussion begin

I cut my pocket with a climbing cut a bit less than half the cutter width each cut ... then do the very last tool line again in the opposite direction.
(a clean up cut)
I generally see a strip of wood that measures about .003" in thickness removed on the that last cut.
It makes a difference as to the way the inlay piece fits into the pocket.

I cut the inlay piece the same way using a clean up cut in the opposite direction. Its is easy to do when generating the G-code in the NC part of BobCad.

You get more cutter deflection with a full width cut than you do with a 40% width cut.

I do not "hog out" a pocket with a larger cutter.
If I want the small radius then I use a small cutter (.0313") for the entire cut.
If it is an inlay like a dot or something with larger radius corners and points I use a larger cutter (.0625").

To adjust for proper fit I always make the inlay .003" smaller than the pocket ... or the pocket .003" larger than the inlay piece to allow for the machine.
Your "number" may differ depending on your machine.


Willee

 

[Tony Zinzola]

I usually hog out the middle first with a .0156" cutter, then clean up the edges both clockwise and counter-clockwise with a .010 or a .012". I leave a .002" edge for the cleanup passes. I'm not concerned about deflection cutting only a couple thousandths off on my cleanup pass and I usually run that pass at about 3ipm. I do the roughs usually somewhere between 10-15.

I calibrated my machine running at 150ipm's and it wasn't missing any steps. As soon as I was done calibrating, I dropped it down to a max speed of 20. I don't want to risk it skipping at any time. With these speeds, I can set an indicator on the spindle that reads to .0001", move the machine 30 inches away in 100 different directions and then tell the machine to go to 0. When I do, the indicator reads .0000. Even with this accuracy, I still get nervous moving too far away. If I'm doing a butt sleeve with a few inlays in the at the same location on the A Axis, I will usually switch my bits several times, getting each pocket done completely before moving on to the next. I also have a quick change spindle, so it takes me just a second to switch bits.

 

[Bill the Cat]

Thanks for the good ideas

Thanks to both Willee and Tony:thumbup:

I was worried about tool deflection with the smaller cutters, but I never thought about cutting twice in opposite directions....duh!!!!!! That certainly should take care of it.

Just a word for Tony. You consider using a .0156" cutter as "hogging"?

Now I know why your stuff looks soooo good:thumbup:

 

[Tony Zinzola]

Just a word for Tony. You consider using a .0156" cutter as "hogging"?

Now I know why your stuff looks soooo good:thumbup:

It all depends on the size of the Inlay. If I can start with a .020 or a .0313 cutter, I do, but I also don't want to have to change cutters more than twice on a pocket unless it's absolutely necessary and a lot of my inlays are so small that the larger cutters will not fit in a lot of the pocket.

Also, if you're using that Wolfgang Spindle, you can go as small as .010, but realistically, I'd probably stick to .0156's. I did some cues with that spindle and the .010's and I broke a lot of cutters.

I did since Friday and almost everything was done with a .012" and I never had to get a new cutter out. I'm running at 50K RPM's though and if I have the music on, I can't tell if the bit is turning or not, unless I look at the controller or put my finger on the depth ring to check.



.