I've built a fixture but I am a little confused on how to locate CNC Zero on it. The machine is a KAFO horizontal CNC Mill (JIS).

I know I need to locate off of 2 reference planes but I'm not completely familiar as what surfaces(ie. fixture plate, fixture base) can or cannot be used to locate zero on the machine. Below is a link to a picture of the fixture I built for reference.

http://img271.imageshack.us/my.php?image=fixture8vq.jpg

http://img271.imageshack.us/img271/7520/fixture8vq.jpg

Thanks for the help!

I program a Mori Seike MH 1000 Horizonal everyday. The pallets are almost 40" square and the parts are rather large. Depending on what the part is, tolerence and who built the fixture, I may either probe the part in the fixture to get a 0 point, probe a stop on the fixture or just go off of the center of the machine table since I know where center is. Their are always many ways to do things.

I highly doubt you built that fixture without ever having to find a zero. Manual or CNC, its the same thing. Edge finders and indicators. A probe if your fortunate to have one.

There is one more alternative, a tooling ball!

All I ever had to do was to ream a 1/4" diameter hole near the front of my fixtures, so the opperators could drop a tooling ball in the hole! The center of the ball is .25000 from the surface of the fixture, so regardless of the angle of approach, the center of the spindle dialed to the center of the ball would give the programmers a perfect starting point!

Eric

I'll go with the reamed hole, used it many times, never used the ball though. Is there an advantage to using the ball versus just sweeping the hole? I've also seen someone sweep a reamed hole for zero, but never check to see if the fixture was straight. So, what is the advantage, I'm curious, I'm always up for some new tricks.

I'll go with the reamed hole, used it many times, never used the ball though. Is there an advantage to using the ball versus just sweeping the hole? I've also seen someone sweep a reamed hole for zero, but never check to see if the fixture was straight. So, what is the advantage, I'm curious, I'm always up for some new tricks.


The advantage of a tooling ball is when your datum is not in a simple location, like in the middle of a bore at a step in the bottom of a hole, or if you comming in at an angle. The trick is to build the fixture around the use of the tooling ball, and trig to the datum. That way the opperator just dials in the ball from where ever the part is rotated. When the CNC programmer has the info, they just program from it.

The shop i worked in did lots of stuff for NASA, Lockheed Martin, Harris, Grummen, it was all goofy hogouts, with the datum under the part a 13.096812763840 degrees from some intersecting bore! All with tight true positions no less!


Also, the tooling balls are super precision, and the ball can give you two axis at one time, not just centerline!

Eric

Master of Widgets, I'm still a little confused. Programming from a random point that you put into the fixture, I understand, but how is the tooling ball a greater asset than a reamed hole or a dowel pin in a reamed hole? I'm assuming its picked up with an indicator, or am I missing something?

Ok, drill your hole, then rotate the head on a bridgepor 37 degrees, and dial in the pin
All you gen is one axis, centerline ....
If you dial in the tooling ball, then you get two axis to a known distance from the center of the ball! Its in the trig! The ball center is constant! I agree this is only usefull if the part is rotated from a standard XYZ position. But on a horizontal pallet mill, the pallets can rotate under the cutter, this is an awsum means to aproach a true datum.

I have had tooling just to hold the tooling ball in a specific point in space, dialed the ball in, then removed the tooling and inserted the blank part!

Not all parts are straight moves in XYZ directions!

Eric


Eric

Hi,
Like Fastoles I use a horizontal(Bridgeport BPC320) and find using the centre of the pallet as my work zero works the best in most cases.
The total Z distance I have from machine zero to the centre of the pallet is 398.96 mm so this becomes my work zero value in the Z ..likewise in X I have total travel of 350mm so the centre of the pallet is 175mm and in the Y the total is 320mm from machine zero to the top surface of the pallet.

ie G56 X175 Y320 Z398.96

I then place my part in the same position on my cad cam and the software does G code correctly.
Ie if the part is 100mm from the centre of the pallet in the Z my Z top is 100. The same goes for X and Y .

The machine control will offset in the plus direction for the length of each tool given in the machines tool library.
Ie if the tool is 100mm long from the gage line, the spindle will actually go to Z200 to accomadate the tool length.


Of course I use an edge finder to position the fixture on the pallet to start with.
Hope this helps!!
John.

I really think the best answer is "It Depends". The machined part configuration can affect this decision, along with if you have the ability to probe internal to cycles. All the parts I machine are fully machined from billet plate, and I do not have probing capabilities. This lends to my preference of using the same datums outlined on the fixture drawings. The fixture was built using those datums, so to me it makes the most sense to use those datums when programming to ensure you know where the fixture features / part locations are. By using the fixture datums, I do not have to deal with locating the fixture to an exact point on the table or maintaining fixture offsets either. I use a G92 coordinate offset which makes my program zero the same as the fixture zero. Many times my fixture zeros are reamed holes / flat surfaces, and that works fine for me. They are easy to locate via an edge-finder or dial indicator, and are easily repeatable each time I set the job up.