Re: [CAD_CAM_EDM_DRO] Going home

Ian Wright wrote:

> Hi,
>
> This may sound like a silly question but where on the 'Z' axis would one
> normally put a 'Home' switch? The reason I ask is because, on the little
> mill I am making, the 'Z' axis, like the other two, has about 6" of travel
> but, like the other two, doesn't move very fast (don't know whether this is
> due to the computer, P266, the motors, 5volt steppers run on 35 volts, or
> EMC, but all the axes are really quite pedestrian).

It is likely due to the motor/driver combination, as EMC should do OK
on a P266.

> I assume it would be
> safest to put the switch at the top of the axis, as far away from the table
> as possible but, if I then have to home all the axes before starting a job,

You only need to home once when you start EMC. After that, it should
stay in sync. If you are losing steps, then you really need to address that,
as rehoming every time you start is really patching up errors that have
already ocurred.

> this could add quite a bit to the processing time. My other thought would be
> to put the home about half way up as the chances are that most machining
> will take place near the bottom of the 'Z' travel. What do you think and
> where is the home switch on your mill?

This should be fine. Although, it is somewhat cleaner to have the home
position at the top.

>
> Another thought is that I am intending to make two or three different cutter
> heads for different purposes - a high speed spindle for engraving and small
> machining, a bigger one for milling etc. As these will undoubtedly sit at
> different locations on the 'Z' axis travel, is there a way in EMC to
> automatically set different zero positions or would I have to set this up as
> a whole host of 'tool length' settings? (I assume I am right in thinking
> that you have 'Home' away from the table but Z 0.000 where the tool just
> touches the table?)

Not necessarily. I usually set Z=0 to the TOP of a part, as this is the
easiest. This is a common practice. Setting Z=0 to the bottom of the
part (could be table, or vise bed, etc.) is also common.

There are 2 ways to do this in EMC. There are tool tables, which are kept
from run to run. You could preset tools into the tool table so the length
will automatically be right. You can also set a work offset for this
variation. The G54, etc. (I think that's the right G code) work offsets
are usually used to offset part coordinates when you have several parts
mounted on a fixture, or two vises on the table. But, it can hold Z offsets,
as well.

One additional concern, is the the tool table and other offsets don't work
well with collets or drill chucks, as the tools do not clamp in repeatable
positions. That is why I have moved over to end mill holders almost
completely in my setup. These will repeatably position cutting tools
if you leave the same mill, drill, countersink, etc. in the holder until it
is worn out. What I have done is make a holder taper fixture that allows
me to measure tool length on a surface plate with a height gauge.
I then enter the DIFFERENCE between a 'master' tool and all others into
the tool table. The master tool's length is written on a chart, but entered into
the tool table as zero. All other tools length is measured, and the difference
between the master and the specific tool is entered in the tool table.
Then, you touch the master tool (I use a center drill as it is the first tool
often used) to the work or other reference surface, and enter G92 Z0.005
(I put a sheet of paper under the tool, and when it is pinched by the tool
I stop jogging down, the Z.005 compensates for the paper thickness).
All other tools will now ALSO read Z=0 when they touch the part.
(You have to be real consistant when you do this, regarding the tool
selection command, or you will end up ramming a drill bit through a block
of aluminum at 45 IPM, like I have done, when I forgot to inform EMC that
I had loaded a new tool!)

Jon