SAME part 2 fixtures ..VMC with no 4th Axis

[kojack]

I have a block with vertical machining operations .. it also has

45 deg holes and a bevel ..


I understand how to setup and machine the top of the part ...

I understand How to change my WCS to the 45 degree face and drill the holes

I understand how to build the fixture and hold the part ...

what I am confused about is where Do i place a new datum for the second

operation.. The part will not have a bevel if it did I would grab the corner

and be done with it ....... any tips or suggestions ..

Thanks ~ Kojack

[kojack]

TT

[cadcam]

Kojack is this the file you sent me if so I will put an example together for you later.
I will do it in X3 if this ok?

[kojack]

Originally Posted by cadcam Kojack is this the file you sent me if so I will put an example together for you later. I will do it in X3 if this ok?

Yea that is the file ...

It doesnt mater what version if its a video to watch .. I dont have x3 yet trying to get the company to foot the bill Im just wondering what to Orgin on the sec operation ...
I will be using the vise for the top of the part g54

I will be using a manual tilt table for the holes and bevel g55

thanks for the help

[kojack]

maybe I should do the bevel first ??

[Donkey Hotey]

This sounds more like a machining method question rather than a Mastercam question. You're going to use a different work offset for the beveling operation, right? Are you having a problem deciding on where to set the origin in the machine (and therefore, in Mastercam)?

[kojack]

Originally Posted by Donkey Hotey This sounds more like a machining method question rather than a Mastercam question. You're going to use a different work offset for the beveling operation, right? Are you having a problem deciding on where to set the origin in the machine (and therefore, in Mastercam)?

yup thats it .. cause when i set the new WCS the TC will be on that 45

but when i fixture the part there wont be anything to indicate on that plane

I have a few ideas but im looking for something to get it close like +or - .002

any tips?

[Donkey Hotey]

Holding a tolerance that tight will be tough. I don't know what the dimensions are like on the part or where that POM .002 needs to reference to.

If it were me, I'd probably machine the plate square, with sharp edges (truing-up the edge where the bevel is going to go). Then on the Mastercam model, I'd trim the edge lines until they intersect, creating the same sharp edge on one corner. Now you have a corner to move the WCS to in Mastercam and a similar corner to touch off on your part.

The reason I have reservations is that the sharpness of that corner will affect how tightly you maintain the depth of that bevel.

A trick I learned from cadcam is that you can use any pair of lines to establish the orientation of your plane (the XY edges of the bevel) then move the physical origin to another point. During the setup, there is a button with an arrow on it. That's for moving the 0,0,0 point to a new position.

Pick two edges on the bevel face (establishing the plane), then move the origin to the imaginary sharp edge above the bevel. Done.

[Matt Berube]

In your first post of this thread you mention a fixture... I believe this is the key.

I would personally design a fixture with a known location to add a "tooling ball". You should draw the tooling ball into your mcx file and create the new angled WCS over the center of the tooling ball.

I do this fairly often and could probably come up with an example if necessary.

For the ball I would recommend Mcmaster-Carr 8481A27

[Geof]

Originally Posted by kojack yup thats it .. cause when i set the new WCS the TC will be on that 45 but when i fixture the part there wont be anything to indicate on that plane I have a few ideas but im looking for something to get it close like +or - .002 any tips?

Plus or minus 0.002 should be easy in one direction but maybe not in the other. From the picture I am guessing that the centerlines for the holes in the bevel must intersect the centerlines for the other two holes.

I don't use CAD/CAM but this part is just flat surfaces and circles so I could hand code it.

I would place a work zero at each of the through holes with the boss and do all the 'flat operations', with the long dimension along the X axis.

Before moving the part I would secure one of Matt's tooling balls into any one of the small (bolt?) holes; if these are tapped that would be very easy.

Then I would 'probe' the ball to find its center location relative to one of the work zeroes. Mr Hotey knows I don't use probes either; my probing would use a coaxial indicator. I really only need to know the center position on the X axis, not vertically.

Now I would move the part to the angle plate and dial it to make sure it is parallel to the machine travel on the X axis and probe the ball again.

After this second probing I can easily set my work zeroes to the centers of the holes through the bevel to within +/-0.001, maybe better because with care my coaxial indicator can give me a bit better than +/-0.0005.

So now I know that my holes centerlines are going to intersect correctly on the X axis.

The tricky part is getting the getting the Y position; looking at the drawing it seems the holes are in the center of the bevel face.

Depending on the precision required maybe these can be eyeballed, but possibly the centerlines for these holes need to pass precisely through what was the original corner before the bevel was machined.

To find this corner to within about +/-0.002 I would grip a tooling ball in the spindle making sure it was running true.

Then I would use this ball to probe the two flanks to the corner I want to locate; this would use my tried and trusty piece of paper.

Bring the ball down to a Z position so it is about halfway down the edge then move in on Y until the paper is just pinched but doesn't tear when it is pulled out; record this Y position.

Move to the other Z and at the same Z pinch the paper the same amount and record that Y; the corner, i.e. the Y for the work zero is halfway between these two Y positions. Fortunately the angle is 45 degrees so trig is not needed.

[cadcam]

Here a a thought for holding and doing the angle after doing the first side in the vise. I can give you the model. I remade your part into a solid from the info you gave.

[kojack]

wow I didnt think of using a fixture like that The male bosses should work Great

Im going to use Bolts to clamp the part ...

Where did you decide to place the setup origin

Thanks Again