Re: [CAD_CAM_EDM_DRO] Setting up end mills for CNC, and other things.

"Fitch R. Williams" wrote:

> I'm working on my first program that will use two different end mills.
> I don't really "need" two, I just want to use two as a learning
> exercise. So I'm programming the machine to make one pass round the
> profile with a 5/8" 4F hogging mill, followed by a 4F 3/4" end mill to
> make a finish cut.
>
> First an observation: I was interested to learn while playing with the
> speeds and feeds calculator that within the constraints of surface
> speed of the cutter (I happen to be using all HSS end mills) staying
> constant, and number of flutes staying the same, when profiling around
> a part, it is apparently faster to use the smallest end mill that can
> safely make the required depth of cut.

It took me a long time to make this discovery! You're doing very well!
The advantage of the big tools is their stiffness. If you are taking very
heavy cuts, or cutting very deep along the side, or need to reach deep into
a cavity, then the larger tools will do it with less deflection. But, for
metal
removal rate, the faster you spin the cutter, the more bites you take.

> Why is this I wondered? I constructed the following answer for
> myself. The smaller mill makes more cuts per second at its given
> surface speed because the cutter lips are closer together for the same
> number of flutes, so it can be fed faster while carrying the same chip
> load (say .002" per lip). I guess this shouldn't surprise me, I just
> hadn't run into it before using a manual mill with an un calibrated
> potentiometer setting the feed.

Now, with really big end mills, you can use a LOT more than .002" per
tooth of feedrate, if the machine is stiff enough to handle it.

> But I am straying away from my questions.
>
> First: Using two tools, I need to pay attention to the differences in
> offset for the two tools. To that end I'm working at learning the
> Anilam's "tool" commands. I am having a bit of a problem with BobCAD
> getting it to program corners correctly (move in an arc centered on
> the corner, radius equal to cutter radius) on the part profile with
> out using an offset path so that when I implement the offset in the
> controller, it will cut where it is supposed to on corners that are
> square or pointed. For example, if I set up an offset tool path it
> will show the cutter centerline moving in a 90 degree arc with the
> corner of the part at the center of the arc when it goes around a
> corner. I'm not so sure I'm getting that except when I use the offset
> function in BobCAD so I can see the path. Is there something special
> I should be doing on corners, or should I just manually take the
> cutter centerline past the edge by a cutter radius?

If you don't use cutter radius comp. on the CNC control, then you need
to construct the offset line, and point to that line when generating the
G-code, not the part outline.

If you WILL use the cutter radius comp on the control, then you don't
construct the offset line, and just make the G-code from the part outline.
BUT, you need to place "lead-in" and "lead-out" points strategically to
allow the machine to follow the proper path when interpolating in
(and out) the radius comp. on the first and last moves. This is an art,
and you have to learn what kinds of moves work best on each control.
The trick is to not make an inside corner tighter than the tool radius,
or the control will flag it as an error. Different controls have different
tolerances for this.

By the way, the end mills work a lot better if you arrange that the actual
curve will be LARGER than the tool's radius. Otherwise, it greatly
increases
chip load during the arc move, causing more tool deflection.

If these comments don't help, send me a message, as I also use Bobcad,
and have done this. I can't fully understand what you are asking about
manually taking the cutter centerline past the edge. But, it sounds like
maybe
you are asking about lead-in and lead-out.

> Second: Do you have any trick ways of setting up the vertical
> offsets? My current plan is to go to the machine, install tool 1,
> move it down to touch the top of the tooling fixture, read the "Z"
> readout. Then do it again with tool 2, repeat for all tools needed.
> Note the difference in "Z" readings form some "standard" and account
> for that by manual programming. Is there an easier way?

This is somewhat similar to what I do. You can make an height block
that has, say, a 1" height, with an insulated flat place on the top, and a
battery and lightbulb (or beeper) in it. When you bring the tool down until

it touches the top, you get a light or beep. The tool is then 1" exactly
above the workpiece. Make your shortest tool (handy if this will be your
first tool, like a center drill) the reference, and call it's length 0.
Now, measure all other tools against that, and enter the difference in
the tool length table, generally as a positive value.

> Third: How do you go about measuring tools in holders so that it
> isn't necessary to re-baseline the tool in the holder by installing it
> and going to some place to touch it down? My number of tools is small
> enough that touching it down to the top of a 1-2-3 block to find out
> where it is relative to home isn't that big a deal, but it seems like
> it would be better if I had a fixture I could put the end mill holder
> in and measure the "Z" offset that was going to need to be in the
> program.

I did exactly that. I made a think that is similar to a cylindrical square,

but it is bored and ground internally to fit an R-8 taper toolholder.
I bought a bunch of toolholders. I rarely take the center drill out of the
holder, so it becomes the reference. I record the length of this tool on
a sheet of paper that stays next to the machine. Whenever I will be
switching tools in a program, or for other reasons will be using length
offsets,
I can measure my other tools, subtract the length of the reference tool,
and enter that in the tool length table. You can see my poor-man's
tool presetter at http://pico-systems.com/preset.html

If I lower the ref tool to touch the work, then do a G92 Z0 to set the
coords to 0, when I mount the next tool and select it, the next Z
move will take the length into account.

Using the tool length offset only sometimes is dangerous, by the way!
I have rammed drill bits into work at 50+ IPM, which is a good way
to break them off DEEP in the work, so it is a bear to get them out.
If you forget to enter the length in the table, or forget to manually
select the tool, then it will assume the tool is the same length as the
ref tool (center drill) and will rapid the tool deep into the work before
slowing to proper drilling feedrate. OOPS! Well, the only answer is you
have to be very methodical about things. CNC definitely allows you
to break stuff faster, too!

Jon