Re: Electric handwheel? Practice notes/thoughts...

-
Kim,
Thank you very much for sharing your real world hands on knowledge
with us. I found it very informative.
Al Lenz

-- In CAD_CAM_EDM_DRO@yahoogroups.com, Kim Lux <lux@d...> wrote:

> 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@a..., timg@k...

> > > Moderator: pentam@c... indigo_red@q... [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@d...>