cnc milling set up

[DBcooper]

hey all, ive got probably a stupid question regarding work offsets and tool offsets. manual machinist gone cnc, so please go easy lol.

currently im zeroing all tools off the face of the part using a 1-2-3 block (looking into tool setters now)

my question is, what do i need to do in order to keep all tool length offsets the same, and just set my G54 Z datum in one shot? i do not currently have probing, just a haimer 3d sensor. im wasting quite a bit of time setting tools that are always in the same holder every time i do a setup. im assuming its something simple, just a matter of getting the right value in the G54. hope all of this makes sense, thanks for your time

 

[couch]

Set all of them to a known/constant height off the table, like a 4.0000" JoBlock for example. Then take your Haimer and zero it on the same block. Zero out your Relative Z-Axis position, then zero the Haimer on the top of your stock, or wherever your WCS Z is and put that Z value that is now in your Relative Z, in your Z-Axis Work Offset.

Ideally you'll use a block that is higher than wherever you are usually running parts, so if you forget to set the Z it doesn't slam into your part/workholding.

 

[DBcooper]

Excellent, thank you for the explanation!

 

[DouglasJRizzo]

Set all of them to a known/constant height off the table, like a 4.0000" JoBlock for example. Then take your Haimer and zero it on the same block. Zero out your Relative Z-Axis position, then zero the Haimer on the top of your stock, or wherever your WCS Z is and put that Z value that is now in your Relative Z, in your Z-Axis Work Offset.

Ideally you'll use a block that is higher than wherever you are usually running parts, so if you forget to set the Z it doesn't slam into your part/workholding.

Exactly how I taught customers that didn't have probing. Very good explanation.

 

[Bobw]

First thing, what does your length offset represent?

It is the distance from your tool tip at the home position to your part.. 99.8%
of the time, that # is negative, because its down (on a 3axis)..

So lets set them all to a common place, lets say the table top (it can be literally anywhere).
So you get 18.000 inches from tool tip to table top for T1. Its a negative #, tool tip to table top,
DOWN, NEGATIVE.. -18.000 goes in the tool table..

Now you toss a part in the vise. And measure from the table top to the Zzero you want
on the part.. And you get 5".. In this instance, the part is above the table top, so that
# is going to go in your G54 5 or 6 or whatever as the Z #... Positive, since it is up
in the instance, if your reference was above your part, it would be negative..

So we have -18.000 in the tool table and +5.000 in the fixture offset.. So if
you take a tape measure, and measure from the tool tip(at home) to the Zzero you want to
use, it will be 13"...

All you are doing is adding 2 #'s.. The hardest part is just wrapping your head around
which direction you are going...

 

[706jim]

Best to set tool offsets positive IMO. Most probes use this logic as far as I know.
And the offsets can stay in memory for years unless the actual tool geometry changes.