Lining up a CNC mill to an existing bolt pattern?

[youngfg]

How would I line a my cnc mill to an existing bolt pattern?
I want to change an existing bolt circle. I want to make the bolt circle larger by making a bigger hole than the orginal, that is offset slightly.

Here is a drawing of what I want to do. Existing part is in black, changes in green.

The part will have a center hole that you could use to line up to, but I am not sure how I would get the part "clocked" correctly.

[nervis1]

Make a fixture that fits the existing hole pattern that is indexed the same as the drawing in the CAM software.

[One of Many]

Originally Posted by youngfg The part will have a center hole that you could use to line up to, but I am not sure how I would get the part "clocked" correctly.

Fasten a sub-plate to the table or clamped in a vise. Drill/ream for the center pilot pin and set this as X,Y Zero then drill a .5-.509 hole at the 3 O'Clock position to the original BC radius. Place the part on the pin and use that .5-.509 hole to clock the original with a pin through the part and the sub-plate. Lock it all down at that point and remove the clocking pin. Now you will already have your orientation established on the center hole and can rework the new BC as required. Use a boring head, bottom cutting endmill or create a path to resize the holes with a smaller cutter.

If the centering pin and the BC holes are not on the same plane or are not through holes. You can still place the part on the centering pin and use the clocking pin in the chuck with the X,Y at the 3 O'Clock original BC. Then fasten the part to the sub-plate. Sometimes you will need to get creative, but the point is to use the machine as much as you can to assist in the setup.


DC

[little bubba]

Not being one to make a fixture if I don't have to and production isn't an issue. I would just clamp her down on a plate, pickup on the center, call that zero and then pick up on one of the other holes, and then write my program from there. I'm assuming this is a one off. For more than one, the center hole and clocking pin seems like a good bet.

[ctate2000]

Thousand possibilities....

I would place on three jaw, indicate center hole and set as zero. Then place dowel pin, drill or other cylindrical part in spindle. From MDI mode call fixture offset and move to any known hole location. Jog tool close to part loosen chuck just enough to rotate part and jog tool in to hole. Snug the chuck up. Send tool home and then tighten the chuck. You can now remachine the part by calling tool, fixture offset and programming a bolt pattern.

[Konrad]

I'm with little bubba

[ctate2000]

My method is a little heavy on set up but will save some program time. If you do not locate one hole at a known location you will have to trig at least one hole to get your x and y coordinates. Having known location for the first hole wil allow you to use canned cycle in FADAL control and no tirg. Like I said there are probably 1000 ways to do this. If size is not critical the fastest way would be a drilll press and ream. Let the ream find the hole and just make them bigger. Simply place ream in the hole with part unclmped and spindle stationary. This will center hole to the tool hold some pressure on the part with ream and clamp in place. Raise tool clear and turn on spindle then ream hole. Whole process would take less time than indicating part on CNC.

[Burgs]

Hi There
We do this all the time and basically do it by ctate2000's way. We try and pick up at least 2 holes though. Been doing it this way for 4 or 5 years and never had a come back or loss of job. Usually we have to do it to fit bigger jobs into the VF3 than we should.
The more you do the quicker you get at it.
Best Regards Burgs

[Pat2000]

Here's another 'lazy' way - put two pins/drills/bolts in your existing job at 1 o'clock and 5 o'clock (I'm reckoning they are both at the same angle from a verticle line on your drg.

now you can use the 'T' slot in your table to align the angular rotation of the job with those two pins/drills/bolts

real lazy way now - LOL pin in spindle located in your center hole gently jog the axis (y axis usually) while feeling the job rocking when rocking stops set X0, Y0 and clamp job down.

you want that waste material under job usually! and you may need that rotation in yer prog.