Re: [CAD_CAM_EDM_DRO] Re: Electric handwheel? Practice notes/thoughts...

I got so carried away on the positioning of the feedwheels that I forgot
to comment on the use of detents and friction devices. I actually think
the gist of this question is about how to quickly and easily manually
machine one off parts with a CNC machine, so I'll go into some detail on
that.

Believe it or not, the knobs (or dials for feedwheels themselves) caused
us a considerable amount of anguish. We started out machining (on the
CNC lathe of course...) nice big beautiful 3.5 inch feedwheels to mount
on the encoders. Although they had a nice tactile feel, they had too
much (or just the right amount) of inertia. They don't stop
immediately... they feel a lot different than a manual lathe feedwheel,
for example. The thing that takes some getting used to is the sheer
mechanical advantage that one has with electronic feedwheels. Case in
point, when setting up insert based lathe tools to touch, you can
literally crush the insert without straining your pinkie. Add a
feedwheel with inertia to the mix and it feels weird. Having said that,
we've still got a steel feedwheel on the X axis of the lathe.

The encoders themselves have some drag, but not much. We are now using
a light plastic 2.5" "finger dial" we found in McMasterCarr. They are
liked by most everyone that runs the equipment. Inexpensive too.

When we first put on the encoders, we thought that we are going to
like/need detents or some friction device. We've found that isn't
necessary. When you run feedwheel encoders, the wheels are only
functioning in jog mode (and in single step run mode with my TCNC3
mods...). Thus, you don't have to worry about bumping them during
production "automatic" runs or during MDI command operation.
Furthermore, they have enough friction that they don't move by
themselves.

I thought we'd need graduated wheels too. In practice this is totally
unnecessary. If one wants to move a precise amount, say 0.010", one
will generally set the resolution of the feedwheel to something sane,
like 0.001" per graduation and then just watch the CNC controller
software until the right dimension is reached. Graduations/detents
aren't needed and probably won't be missed.

Truthfully, the thing that feedwheels are used the most for is tool and
workpiece setup and they are indispensable for that purpose. I find it
very slow to zero workpieces and tools with code commands especially
when one is trying to touch off an edge, diameter, etc. As far as
saying that you will machine a surface (or diameter) via the feedwheels,
I don't think you will. ***IF*** you have a good single step/jog/MDI
user interface, you'll issue a g1 z-2 f6 before you will stand there and
turn the feedwheel for 20 seconds. Once you learn Gcode, it just
becomes second nature to issue a command and let the machine do it.
Ditto for using the mill. In spite of having the quill available for
drilling, I rarely drill holes manually or with the Z axis feedwheel.
All our holes are drilled with:

g98 r0.25 ; set the Z retract height
g78 z-1 i-0.1 f1 P200 #1000 ; stop for a second above the work

BTW: we've implemented symbols in our version of TCNC. Ie we can issue
the following on the commandline in *jog* mode:

%hole1 = x1 y1

This sets the symbol %hole1 to equal "X1 Y1" in any Gcode command. This
is extremely handy when MANUALLY machining something using GCodes.

Actually, I usually don't use the symbol "%hole1". I'd use "%h1" or
even "%1" because it is faster to type. I can then type "g0 %1" and the
machine goes to hole 1.

The other thing that is very handy is to have HISTORY, ie whenever you
type in a command, it is available for re use via a scrolling history on
the MDI command. Thus, my sequence for drilling and tapping 4 holes is:

a) enter the hole locations:
%h1 = x1 y1
%h2 = x3 y1
%h3 = x3 y3
%h3 = x1 y3

b) move to the first hole
g0 %h1

c) put in the center drill and set Z0. I usually let the bit rest on
the work and tighten the quill lock.

d) Issue a simple drill command:
g98 z0.25 ; set the Z axis retract height.


Why use G78 when I only need a G1 for such a simple hole ? Two reasons:
a) it handles retracting the bit away from the work automatically, so I
don't have to type in G0 z0.25 after every hole and b) we are going to
reuse the command later.

To drill all the rest of the holes, bring up the MDI, cursor to G0 %h1
and edit the line to read G0 %h2, %$h3, etc. This will also save them
all to history... Don't forget to G0 Z0 to get the bit to the starting
point, although it will drill the hole if you don't... you'll just be
waiting while it drills the first 0.25" of air !

e) Now that all the center holes are drilled, drill the real holes.
First go to hole 1. DON'T type in G0 %h1, because it is already in
history... be lazy and cursor up to the command and then run it.

To actually drill the hole, bring up the G78 command we already have in
history and edit it to be the real hole command:

g78 z-1 i-0.1 f0.5 p200 #1000

Run it to drill the first hole. Bring up G0 %h2 to drill the second
hole, G%h3.. G%h4 for the fourth hole.

I find that I use my time while the machine is running to get tooling
ready for the next operation, to measure things, check my drawings,
etc. Also: we've got a VFD on the mill and TCNC have variable feedrate
control, so I usually adjust the two so that the drill is running just a
bit faster than what produces a continuous chip... continuous chips
fling coolant all around and make a mess.

f) Now we need to tap or holes, using a center point in the collet to
center our tap. I change to the center point, reset Z to something that
works with the tap (either via the feedwheels or via a G0 Z1 command...)
and go to work tapping the holes. The quill is free (ie not CNC'd) on
our mill, so I just leave it loose to keep the tap centered. I use
CURSORS and the commands in history (ie G0 %h1...) to move around to the
holes.

I find this method of drilling holes faster than sitting down with a CAD
system, faster than manually writing a GCode file, faster than using a
mill with a DRO and about 5x faster than using a mill without a
DRO.

Of course we'll be replacing the manual tapping with rigid tapping in
the near future.

We use similar routines/procedures on the lathe.

We've written a bunch of non standard canned cycles so that things like
hellical milling, thread milling, tapers, threading, slot milling,
surfacing, etc. are all single commands. Our machining productivity has
improved 5x over using a manual machine.

The other secret to manually machining a part is to start with a
dimensioned drawing. It doesn't have to be CAD quality. We keep these
drawings for every part we make. I usually write the commands that I
use for making the part on another sheet and staple them together so I
can make another one someday. We've got files of part drawings and
Gcode commands all ready to make another one someday.

About the only thing we write GCode files for are production parts or
parts made in quantities of more than 2 or 3.

Our version of TCNC allows us to add commands to the partfile we are
running as it is being run. If we are making up a part "on the fly" I
open up a dummy part file with the headers, etc in in and start adding
commands and then editing/running them. By the time I've got my part
made I've also got my partfile done. I still find it faster to write
the part file first and then run/edit/refine it. There is something
unnerving about writing a partfile with the chuck spinning the part at
2000 RPM... although we can start and stop the chuck at will while
single stepping through part files.

About the only thing I machine manually via the feedwheels is sometimes
I will face a piece in the lathe, on one offs, I will knock the corners
down and I will sometimes feed the center drill (mounted on the cross
slide of course.) I do everything else via Gcode from an MDI command on
our modified jog screen. I use the feedwheels extensively during
setup.

I ask those that have criticized my contributions back to this group to
consider the length and depth of the emails I wrote today.

Kim

On Mon, 2003-12-01 at 13:32, Kim Lux wrote:
> On Mon, 2003-12-01 at 12:17, Graham Stabler wrote:
> > Odd question, where do you mount the wheels?
> >
> > In conventional positions or together?
> >
> > Also do you add some sort of simple friction device to stop over
> > spinning?
>
> These are NOT "odd questions". I had the same questions when we put the
> feedwheels on our machines. (We actually have them on 3 machines.)
>
> On the lathe, we thought about mounting them on the carriage, but then
> decided to mount them right where the screw cutting gearbox levers
> *were*. (We removed the levers, although we left the gear box intact.)
>
> This puts them on the headstock, right below the spindle gear selector
> levers. The idea is that they are right by (actually to the left of)
> the chuck for quick positioning of the tools when setting up tools,
> parts, etc. Incidentally we mounted the monitor on top of the
> headstock, at eye level when standing. The keyboard (sans mouse lately)
> is right below the feedwheels. We find this positioning quite
> convenient. Everything (monitor, keyboard and feedwheels) are right at
> your disposal. *IF* we did a lot of work on long pieces (20"+) we might
> find the controls too far from the middle of the lathe, but as we use it
> right now, it works quite well.
>
> BTW: Our neighbors have a commercial CNC lathe with the control on the
> rightmost sliding door and only one feedwheel. They are not happy with
> that arrangement.
>
> On the mill, we've got the feedwheel mounted at the front, right below
> where the manual Y axis feedwheel was. We've got a lip over the wheels
> to prevent coolant from dripping on them.
>
> We need to do more work on our enclosures. We've got issues with
> coolant and metal chips flying everywhere.
>
> Kim
>
>
> > Thanks
> >
> > Graham
> >
> >
> > Addresses:
> > FAQ: http://www.ktmarketing.com/faq.html
> > FILES: http://groups.yahoo.com/group/CAD_CAM_EDM_DRO/files/
> > Post Messages: CAD_CAM_EDM_DRO@yahoogroups.com
> >
> > Subscribe: CAD_CAM_EDM_DRO-subscribe@yahoogroups.com
> > Unsubscribe: CAD_CAM_EDM_DRO-unsubscribe@yahoogroups.com
> > List owner: CAD_CAM_EDM_DRO-owner@yahoogroups.com, wanliker@..., timg@...
> > Moderator: pentam@... indigo_red@... [Moderators]
> > URL to this group: http://groups.yahoo.com/group/CAD_CAM_EDM_DRO
> >
> > OFF Topic POSTS: General Machining
> > If you wish to post on unlimited OT subjects goto: aol://5863:126/rec.crafts.metalworking or go thru Google.com to reach it if you have trouble.
> > http://www.metalworking.com/news_servers.html
> >
> > http://groups.yahoo.com/group/jobshophomeshop I consider this to be a sister site to the CCED group, as many of the same members are there, for OT subjects, that are not allowed on the CCED list.
> >
> > NOTICE: ALL POSTINGS TO THIS GROUP BECOME PUBLIC DOMAIN BY POSTING THEM. DON'T POST IF YOU CAN NOT ACCEPT THIS.....NO EXCEPTIONS........
> > bill
> > List Mom
> > List Owner
> >
> >
> >
> > Your use of Yahoo! Groups is subject to http://docs.yahoo.com/info/terms/
--
Kim Lux <lux@...>