Tombstone Machining

[Justin Beebe at Folsom Tool]

I am new to horizontal machining and tombstones. I was going through the WCS tutorial example 4 for tombstone applications. I completed the tutorial and machined pockets on all four sides of the tombstone. It posted with a G54 B0 for front face; G55 B90 for right side face; G56 B180 for back face; and G57 B270 for left face.My question is if I were to set this job up on a horizontal mill where would I set G54,G55,G56, and G57? When I press F9 to view the origin it is on the front face lower right corner of the tombstone. Do I need to set a different fixture offset for each face? If anyone is familiar with this tutorial let me know. Thanks..........

[Guest SAIPEM]

The easiest method, in my opinion, is to program EVERYTHING with the center of rotation as the origin.

 

This means that all work coordinates will start out with the same values for X,Y and Z if you only program a 4 face tombstone with a single part on each face.

 

If you have multiple parts on a single face then consider using G54.1 P1-P48 and establishing a separate workplane (Toolplane), for each part face, that references the center of rotation.

[Justin Beebe at Folsom Tool]

That makes sense thanks

[Rick Henrickson The Boeing Co.]

center rotation is a greta way to program, but if you have very tight tolerance on 2nd op multiple parts you will need to create seperate coordinates

[Guest SAIPEM]

Rick-

 

You can still use different Work Offsets it's just that the values that they start with are the same.

 

With tweaking for first article they'll probably change slightly.

 

Multiple part faces would typically have different Y values in the WO.

[Mcam Nut]

I agree with Saipem, I started out programming off the corner of each part, and now I always go off the center of rotation. This make it alot less hard on the head when machining angles, or using the 4th axis to surface. We also have separate offsets for each part, but the z, and x are always the same. I think this way is also alot easier for the operator to setup. we dont use g54-g59 we use g54.1 p1-p48.

[Jack Neelands™]

i will put some old files one the ftp site for you to get a look at ...just have to convert them to X tomorrow

[S.Hall]

The center is usually the best. I have found that if you are using a b c or, u v w axis moves, a seperate offset for each can be helpful if the rotation about the axis has slop problems. Using the degree ,minute, second can help with tolerence issues also. Great post. S.Hall

[Jack Neelands™]

now converted and zipped for ya to look at in the X folder...zipped file is called S00B04D.prt.zip and has 4 examples of hydraulic manifolds programmed with the tombstone as the center but allow for offsets to be changed...just make all the coordinates the same in the machine and move if necessary...ie g54.1 to g54.12 are all the same but g54.13 needs a few thou up for some reason

[Jack Neelands™]

cncjb did you get the files?

[Justin Beebe at Folsom Tool]

I did get the files I went on vacation sorry it took so long to get back to you guys. Thanks for all your help. I'm sure the files will help.