O/T Horizontal Mill

[TheePres]

Would like your opinion, on how you approach work zero position on horizontal mill work. I understand if doing say a housing or valve body that "X" and "Z" zero point would be center of table. But when working on tombstone with part not rotating on cline, do you stack up plate dimensions and shift part to actual location, or do you add tooling ball to fixture and have operator pick up location at each rotation?

[Hardmill]

quote:

---

But when working on tombstone with part not rotating on cline, do you stack up plate dimensions and shift part to actual location

---

If you shift your part (in MC) you only need

to pick up your -Y-, when you rotate you already

know where it is. At least MC knows. No need to

pick up unneccessary offsets. X and Z is center

of rotation.

Hope i'm reading this right.

 

PEACE

[mayday]

It all depends on how you standardize your setups.

some machines have the ability to calculate rotational offsets based on X,Y, origin and angle. I most always gram to print X,Y zero then I pick the outer most surface for Z zero, for safe Z clearance moves. on complex angle gramming I use center of table for X,Z zero but you need to duplicate in MC how the part is set up on the machine. if you dont know where the part will be on the table you will have to calculate the offsets yourself. there's lots

of ways to do it. I like to use the easiest way is for the operator. where it can screw ya is on fabs or castings when a surface needs to be bumped in or out due to stock. that changes everything. I always add in spot cycle for part

qualification cause we dont have a probe on one of the machines. the problem with using center of table is if the part dosnt wind up being where it should for whatever reason. then the offsets have to move anyway 90 deg work is easy. we have keys on 5" spacing and use fixture blocks for setups so we allways know where the part is relitive to table centerline.

[KCollins]

We do the same here as mayday....We always use print zero on the part. We'll make the best approximation using the cast locators and an edge finder to pick it up on the part. Each rotation or tombstone has its own location...ie, G54, G55.....G54.1 P1...When your working with really close tolerances its hard to position the part exactly at the centerline of the table unless you're working with something round or have a locator hole that you can indicate in....

[Mgrenier]

Hello all,

 

Here, we have about 20 horizontal mills. What we ended up doing is to write a custom macro on the machine that will calculate the position of one specific point whatever the rotation angle you want. That saves us a lot of setup time since we do a lot of very big parts

 

Have a nice day,

[mayday]

Martin, is that macro somthing you would like to share???. I have worked on doing that but never came up with a good macro to do it

[robk]

In here I never have any of the parts on the center line of the tombstone...I have a solid of my tombstone as a background for a reference location of the part. It comes in handy especially when doing fancy angle work (I could see if the head of the machine will hit the part or the tombstone in backplot). If there are same parts on 4 sides I will make a main program and run sub-programs. We use a a Renishaw probe to locate the parts. All put together, it works perfect

 

Rob

[specv]

We always use part zero for the program, and use said angle macro to figure the x,y,z coordinates of the other indexes.

 

Pete

[Bob_Looney]

I drew a wireframe of my tombstone, and always used cl of tombstone for X and Z zero. I used local workplanes for programming the part.

Only problem is the part needs to be located as it is in the wireframe. We usually used dowels for locatong second op parts or a couple edges that we machined in op1.

[TheePres]

My current project has 12 different positions and would prefer to use the 1 work offset "G54" at center of rotation, any other method would be to time consuming for set-up people. In my favor is that part starts of as plate. This macro idea sounds great, does this require probe?

[Tim Johnson]

I also find part zero and let the angle macro do the rest of the work. I also create work location programs so the zero point(s) won't have to be found again on the next setups.

[Guest CNC Apps Guy 1]

For me it really depends on what I am doing. I use both methods; C/L of Rotation and locations. I find I have more flexibility if I move off positions though for the most part.

 

JM2C

[mayday]

Theepres, your best bet is to do what makes sence to you, that way you can explain it to the machine guys. if theres a problem,makes it easier for you to fix. if your opp guys need to tweek it doing a lot of trig is time consuming

[Jimmy Wakeford from Barefoot CNC]

Alot of shops set a work offset to each part location. You can grab the numbers in the post and have the program set them with macro b or you can use g10.

 

JImmy