How to find program zero?

[Ashish B]

Hi,

I have a cylindrical part at hand. I have to perform a profile machining operation on it. To accomplish the same, i need to tilt the part by 5 degree.
I will put a fixture beneath the Cylindrical job which will automatically locate the PART in a inclined position.

The problem to me is how to find the Program Zero (CENTRE OF CYLINDRICAL PART) as the PART is in inclined position.
If it is not parallel to XY Plane & not vertical, the how I should find the Program Zero.

ANY SUGGESTIONS.

ThANKS
Ashish

[christinandavid]

Coburg Product Details - Tooling Balls (Standard - 1 Piece)

We used to use 'tooling balls' as a reference point for angled set-ups. Just ream a hole in the fixture to accept the ball, then clock the ball once the job is set at the required angle.

You can then use simple trig to set your datum to a specific point on the component, or if running an offline program set the ball position as XYZ zero on the machine and also the CAM model.

DP

[Ashish B]

Hi

Are you referring to the setup which is mentioned in the attached document?

The Program zero is set at ball centre. By clocking, centre of ball is derived & the real X0Y0Z0 is found.
Am i Interpreting it right?

Thanks
Ash

[christinandavid]

Yep, that's the idea.

For a cylindrical part the convention would be to put the ball on the centreline of the fixture, but sometimes it is more practical to put it in a different position if you need access to it while the component is clamped to the fixture.

Obviously, once your work offset position is established, you can put reference faces/holes in fixture true to the set-up angle, to ease future set-ups...

DP

[Ashish B]

Great IDEA !

I got it about X & Y locations, but how we can set Z offset. You can see in the attachment, that cutter will touch the high point of tooling ball. Certainly, this high point cannot be considered as Z0,

ANY IDEAS

[christinandavid]

Yes it can be tricky to set Z with an end mill, as the end lip is not ground flat - but should be reasonably accurate.

For ultimate accuracy I suggest you use a reference tool or 'gauge length' tool.

You can purchase a bar ground to a specific length from the taper gauge line, or simply use the plain ground back-end of a carbide tool in a collet chuck.

Touch on the ball with this plain bar, using a more 'robust' feeler-gauge. Once you are satisfied, note the machine 'Z' position and minus the combined width of the feeler gauge and radius of the ball to set Z offset to the ball centreline.

DP

Edit: If you don't use a reference tool as standard practice, or if you have many tools to set, do what I mentioned previously and machine a reference face once you are set-up at the angle.

You can use a DTI to check the Z position of the face to the ball centreline - and set your tools accordingly.

DP

[Ashish B]

hEY, That pretty nice.. But somewhat tricky because of the point contact of the tooling ball & the cutter.

For some accurate purpose, we do keep a reference block at the corner of table & set zero over there.
In our case, the X,Y position will be the ball centre, but the Z zero would be top face of refrence block.

I hope you get my idea.

Thanks
Ash

[christinandavid]

Okay, so set all your tools to the block then depending how you operate adjust the work or tool offsets by the distance between the centre of the ball and the reference block.

DP

[Ashish B]

Hey christinandavid

Thanks for your wonderful, superb trick for angled setups.

[christinandavid]

The tooling ball method is most useful when you have a component that requires multiple angled set-ups - especially when these set-ups need to be manually set on angle plates/rotary tables to a high degree of accuracy.

Now, if you have an automated 4th axis, and a little room for error, there is a much better trick called 'dynamic fixture offset'....

DP

[Ashish B]

I really acknowledge & appreciate your knowledge about setups, angled setup.

It was nice talking to you.

Thanks
Ash