g-speed wrote:Thanks for your help. The machine now does something. Next problem!!! When I home the machine the x axis does not read zero! The z axis does read zero and I have cleared all tool offsets and work shift offsets. X did read abot 155mm with a work shift of about 11mm. When I cleared the work shift back to zero it then read 144mm.
All depends on how you want to work on your machine as to what you now do with your work shift offsets, there a few ways you can proceed but here is how I have my machines working to suit how I use my CadCAM software and how I like to work. May not be to the liking of all and may not be right to some of the "purists" around but it works for me!!!
I use the face of the chuck as work Zero and have measured the height of the jaws so I know exactly where I am likely to hit something!!
This means in my CadCAM I can set stock and the drawing correctly so it is clear of the chuck.
I put a piece of ground bar in the chuck that I knew the exact diameter of and set my first tool to that in the X axis and set that number plus the rad of the bar as a minus ( It is -38.44mm ) in the X workshift.
Then used a tool setter against the face of the chuck to get the distance from the home position to the chuck face and put that number in as the Z workshift ( It is 201.58mm ).
So now when I first switch on my machine it will show X 0.00 and Z 0.00, after I "Home" my machine it will always show X107.56 and Z201.58 on the position screen and the machine position is shown as "Absolute" X107.56, Z201.58 and "Relative" U107.56, W201.58 and the Machine position as X0.00, Z0.00.
After that all I do is check tools against the same piece of ground bar but any bar you can measure the exact size of will do and use the tool setter off the chuck and put the offsets into the tool offset library.
After that it`s only a matter of calling a tool number and offset number up (eg T0101 or T010101 if using tool nose rad) in the code and presto the right tool will always go to the right place ( That`s the theory anyway and it`s worked so far for me!!! )
Sorry if some of this seems to insult your intelligence but I have no idea what your level of expertise is so I thought I`d just go through what I did with my machines.
After that I modified a couple of Post Processors in my CadCAM software to get the exact code needed for the 2 machines as they do use some different "G" codes for some operations!! (eg One uses G28 for reference and the other uses G50, all good fun!!) Your Denford Manual should have a list of "G" and "M" codes assigned to your particular control.
After having said all that there is a way to have everything actually reading 00.00 on all axis at "Home" position by setting a Parameter in Fanuc to make this happen but unfortunately I have no idea which parameter of the hundreds in there to change or what to set it to anyway!!
You will have to remember that if you do get all axis to show 0.00 at "Home" position then you need to call up your work shift/coordinate position in your program.
I don`t have to set that in my programs.
Boy, that was some "ramble", hope it all made some sort of sense for you!!
Regards
Rob
.