Bobcad 24 Pocketing Tutorial

It bothers me to rough cut with small cutters. I love efficency!
I use .05 cutters for the vast majority of my cuts. I avoid burying the small bits on cleanup passes by creating extra pockets in the areas that the bigger bits don't reach.
I mislabeled this pic, I was actually using a .03 and an .02, but you'll get the idea...
attachment.php

20ipm for the .03
6ipm for the stepped cuts
12ipm for the finish cut
 
Tony Zinzola said:
I don't run into that problem Bill, but I am using very small cutters to begin with. Right now, I'm cutting out a ton of silver parts and I'm roughing with a .015" cutter and cleaning up with a .010". I had a huge area that the .015" cutter wouldn't fit in, so on the cleanup, I slowed my feed rate down to 1. That works for me. It might not work for you. Your spindle doesn't have the RPM's that mine has and I don't know what sort of tolerances your machine can hold.

What I would do in your case is rough cut with the larger cutter, but leave the side allowance at .005 or even .010". Don't program a finish pass, just leave it blank.

Then do a profile cut on the inside of the pocket with your finishing cutter. That way, on the rough passes, you can leave a .001" side allowance for your step cuts and finish up at full depth without breaking the bit.

I'm assuming you know how to do a profile cut already.
Click to expand...

Thanks for the idea Tony! I really admire your work and appreciate your help!
 
Bill the Cat said:
First, let me say that your generosity in providing this tutorial is without measure!!!!!

Now for my question.

You stated that you make your roughing passes in steps and your finish pass at full depth. I tried that initially, but ran into problems when my design had a feature with an acute angle. I rough with a larger cutter and finish with a smaller diameter. At the root of the acute angle, my finish cutter would be in full cut because of the difference in the size of the cutter used for roughing. The result was that I broke a lot of small (i.e. - expensive) cutters. I could eliminate the problem by using the same diameter to rough and finish, but I like to use the less expensive cutters to hog out the majority of the pocket. I've since changed my finish passes to be in steps (like the roughing passes) and that solves the problem and the pocket wall is still smooth (no step marks), but I'd much rather do my finish pass at full depth. Just curious if you ran into similar problems and, if so, how you delt with them?
Click to expand...

Bill

Sheldon's approach works great when you have a pretty large area between the large rough cutter and the smaller finish cutter.

Another thing you can do is to reduce the "Arc Slowdown". On 23 you find this in the tool window where you set the feeds and speeds. If you slow it down, say 70% instead of 100%, you will get a reduced feed rate on any arc. So when your cutter is in those tight corners, it will go slower and reduce the chance to break the bit.

Royce
 
Tony Zinzola said:
It all depends on the size of the parts and pockets. Most of my parts are very small. I couldn't fit a .050" cutter in most of them. I have also given up on efficiency. I am not a production cue maker. I know that anything I make is going to end up under a microscope at some point, so I will spend days to put a single inlay into the cue if that's what it takes.

Most of my pockets are only .045" or so deep. When I'm doing a bunch of very tiny parts that I know are going to be hard to handle, I first do a rough cut much deeper with a .030" cutter. Then I will do another rough pass with a .020" cutter and then finish it up with the largest cutter I can fit, which usually ends up being a .010 or a .012".
Click to expand...
I'm the same, I do custom orders exclusively.... I strive for efficient cutting not because I'm in a hurry, but to minimize run time on my machines. ;)

I know exactly what you mean about test fitting stuff taking lots of time... That's where the real work is, since there are so many variables that will affect the size of the parts and pockets. Sometimes I wish what some guys say about cnc was true, that you put the cue in the machine and then go get coffee, come back and it's done!

Great work, and thanks for sharing! :thumbup:
 
RBC said:
Sheldon's approach works great when you have a pretty large area between the large rough cutter and the smaller finish cutter.

Another thing you can do is to reduce the "Arc Slowdown". On 23 you find this in the tool window where you set the feeds and speeds. If you slow it down, say 70% instead of 100%, you will get a reduced feed rate on any arc. So when your cutter is in those tight corners, it will go slower and reduce the chance to break the bit.
Click to expand...
The same approach works well in smaller stuff too, unless the size of the cutter you start with is really close to the cutter you finish with, then the extra pockets aren't always necessary. It depends on how steeply angled your areas that need finishing are.
Great advice on arc speeds.
Arc feedrates can sometimes be adjusted at the controller too.
 
Thanks!

RBC said:
Bill

Sheldon's approach works great when you have a pretty large area between the large rough cutter and the smaller finish cutter.

Another thing you can do is to reduce the "Arc Slowdown". On 23 you find this in the tool window where you set the feeds and speeds. If you slow it down, say 70% instead of 100%, you will get a reduced feed rate on any arc. So when your cutter is in those tight corners, it will go slower and reduce the chance to break the bit.

Royce
Click to expand...

I actually had planned to use Sheldon's approach for things like the tip of a floating point. In cases like that (where only the tip of the point is the problem area), I agree it is more efficient to program an "extra" pocket at that point.

The "arc slowdown" sounds neat, but isn't as easy an option for me. I'm using BOBCAD V19. Although I can manually edit my gcode to change the feedrate for any specific move, that option would not actually help in my case. The problem areas I encounter are not arcs. I design my inlays for the diameter of cutter I will be using. For example, if I'm using a .025" diameter cutter for finishing, the inside corner on my inlay will be .0125" using the cutter itself to form the radius of the inside corner. Therefore, the final pass in my gcode (where the problem occurs) is a point-to-point move rather than an arc. In the floating point example above, that move may be from the base of the point to the tip and I don't want to reduce the feedrate on that whole move.

So, depending on the size of the inlay, I'll use either Sheldon's or Tony's suggestions.

As always, thanks to everyone for their input!
 
Nice tutorial Mr. Zinzola, and thanks for taking the time to make it.

From a machinist's standpoint, I see two things that could benefit from addressing.

First, the radii that you are using for the fillets should be just slightly bigger than than the radius of your cutter to avoid parking the cutter the in the corner.

Second, how come you are "conventional" milling instead of "climb" milling? Climb cutting lets the cutter take a full chip load, and will not only cut cleaner, but also increase your tool life.

Please don't think I'm am criticizing your work, as I think you make some of the nicest cues there are. The way you run your operation is clearly working very well for you. It's also cool to see some screen shots of V24. It looks like they have made some nice improvements since V23. Thanks again for taking the time to make this post, and helping some folks out.
 
Bill the Cat said:
The problem areas I encounter are not arcs. I design my inlays for the diameter of cutter I will be using.
Click to expand...

Could you design the pocket using two small 0.1" lines collinear with the sides at the point of the "V" and just slow the feed on those two lines? Does that make sense? Like a 4" V, but one line drawn 3.9 and another for .1 at the same angle on each side.
 
PolarBear said:
Could you design the pocket using two small 0.1" lines collinear with the sides at the point of the "V" and just slow the feed on those two lines? Does that make sense? Like a 4" V, but one line drawn 3.9 and another for .1 at the same angle on each side.
Click to expand...

PolarBear, this method may work but would be hard to set up in Bobcad with different feed rates. Too much work. Most of us are using Mach 3 to run our machines. This issue can be handled in two different ways. The first is to control the ACC/DEC of each axis in motor tunning. That is when an axis starts and stops to move, you control how fast it change speeds to or from feed rate. The other is to change the current mode that Mach 3 is in from CV or constant velocity mode to exact stop mode. You can change this in the Mach 3 general configuration or with G-code. G64 CV or G61 for exact stop. To fix these issues then I would use the 61 to stop axes movement after a movement then the next line of G-code will run.

Jim.
 
My $.02

In response to the past posters:

PolarBear - Breaking the geometry to allow a feedrate change on the last portion of the cut IS possible, but cumbersome. In addition, it does not really solve the problem. When a larger cutter is used for roughing, the amount of stock left for finishing becomes greater at the base of an acute angle. Slowing the feed rate does not change the fact that the smaller finishing cutter ends up being "buried" in cut at the base of that acute angle (rather than taking a small "cleanup" cut). Trying to do this at full depth (even with a reduced feed rate) will often generate enough force to break a small cutter. One of the biggest problems with very small cutters is chip removal. If the cutter is placed in "full cut", there is so little room for the chips to be expelled, that the cutting force goes through the roof and the very small cutters just can't take it.

Mc2 - I, personally, use Constant Velocity mode. I believe this allows the cutter chip load to be maintained closer to it's programmed value and will extend cutter life. In exact Exact Stop Mode, the cutter is at zero chip load (which will tend to burn the cutter) at the start of each move. In addition, if the moves are very short (as in an extremely small inlay), the cutter may never reach the desired chip load at all (depending on the accel/decel settings).
 
Last edited:
If there are sections of a toolpath that you need to maniplate the programmed feed rate you could program a FRO (feed rate override). That allows you to control your feed based off of a percentage of your programmed value. It's helpful if there is an area of code that needs to run slower than programmed, or if a machine can't hold tolerences because of rigidity or power problems. Bill the Cat hit on a good point though. Tools will not last or cut as well if they are run slower than they are designed for. It's all about the chip-load.
 
What program(s) are you using to draw your pictures? I like that Fleur De Lis. I am new to BobCad but not really CAD (but its been a bunch of years). One way I can see to make that right now is to draw it out on graph paper, find the approx center of all the radii, do each entity individually, trim, mirror and chain. BobCad seems to be good for making the pocket geometry and generating the code, but the editor is a little lacking.

What I want to be able to do is draw a basic shape, then drag, pull, crop, extend, widen, bend, curve, add to, etc. the shape without a lot of typing. And if I don't have to really read much documentation, that's a definite bonus.

Right now I am using BobCad V21. But, a friend has V23, the tutorials and the dongle that he isn't using so I may go borrow that indefinitely.
 
Bobcad

Tony,
thanks again, And thanks to Jim Babcock too.
As usual you are overly generous with your time and knowledge. I hope any users and future users of Bobcad can appreciate both of your efforts. I certainly do.
thanks again, JerseyBill
 
Last edited:
You must log in or register to reply here.
Back
Top