Need Help!- How do i get the Fadal to show my zero position instead of its home position?

[DSUDS]

I have a Fadal VNC 4020 with CNC 88 HS control.

When i pick up zero it reads from the machines home postion and shows the cordinates on the screen from its home position. I want the controls to show the numbers from my zero pick up position.
Thanks.

[Neal]

When you apply the fixture offset, the axis will re-zero to reflect the position of the new temporary home. The program will be executed from the fixture offset zero position.

Neal

[DSUDS]

Originally Posted by Neal When you apply the fixture offset, the axis will re-zero to reflect the position of the new temporary home. The program will be executed from the fixture offset zero position. Neal

I know this and dont have any problems with my programs but.......


If i am picking up two holes which one will be zero and the other will be my rotation point then my numbers i need to plug into my software are different.


Example : My zero postion is zero for my software but the machine postion is x-5.00 y.250

then my other hole is machine position x .9620 y.685

I have to go back and figure out what numbers to plug into my programming software.

I'm just wondering if there is a code i can punch in my mill to work off of my zero while i pick up my part then go back when i run my program.

[FastFieros]

There is 2 ways to do this. One is the ZERO at part way. The other is to use the Fixture Offsets.

ZERO AT PART:
Use whatever method you use to index to the center of that hole. Do a SETX SETY . There is also set zero X Y Z on one of the selection menus at the bottom, but I cant remember which one it is right off.

After you do the SETX SETY , that is your new position ZERO. Work with the coordinate plotting you need to. Run your program from here as your home ZERO. I dont recommend you setZ as there is no real need to move Z from the CS zero so the ATC will react correctly.

Once you run that program that you want to do this zero to on the part, do a HOME AXIS for power down. That will return the Axis X Y Z to the CS zero. IF you are not ready to power down the machine, just do a SETX SETY again and this will relocate your X Y back to the machine CS zero position.


ZERO machine CS, ZERO using fixture offsets:

What Neal and others on the forum prefer to explain as better coding and working with machine zero is to learn to use the fixture offset screen.

I use Mastercam. I know your pain in seeing the numbers on one thing over the part, and you are expecting the same numbers you see in MasterCam, of whatever you are using. Here is another thing I do to get around this because I now use the fixture offsets only for the most part.

Get the offset to your part ZERO. I usually work around the center of the part if I can, or create an index hole. Once I know my fixture offset for lets say E8 is X2.00 Y3.00 My tool is headed to my zero of my part. Now, the screen is showing that X2 Y3 deal and not X0 Y0 .. However, if you hit auto and start the program running, and then do a slide HOLD, the zero on the screen is your X0 Y0 location and it shows this on the screen. In slide hold you can select to JOG, and do all the plotting and checking you want with the numbers showing exactly what you want to see compared to your same numbers in your software. When you come out of slide hold with lets say Manual, you are back to the offsets numbers, so watch out for this.

Wow, I hope that is understandable.

[Fadal Error]

Originally Posted by FastFieros if you hit auto and start the program running,

You don't have to start the program. Just go to MDI mode and enter "E8 G0 X0 Y0 Z0" or whatever position you want. Then you can push the jog button and move to any position and it will work off of that work offset. If you push Manual, you will cancel that fixture offset and it will display the machine zero or E0 coordinates again.

Try it without a tool in the spindle at first to be safe.