Please help with part alignment when flipping parts!

[momospeedracer]

The problem at hand is aligning the part after flipping it for bottom operations.

For example, I want to make a 2 x 2 x 1/2" square piece with 1" hole at the center of the part. Top and bottom are lightly chamfered.

I'll start off with a 3x3x1" stock, eyeball the origin at about 1/2" x 1/2", face the stock and profile down 1/4". Run the chamfer bit on all all sides.

Everything comes out nice and even - so far so good.

I flip the part and clamp it into my vise with machined soft jaws with a profile of the finished part.

This is where I'm having trouble aligning the part. The only reference points that's obvious to me are the edges of the square hole in the center of the part. I find the center of the part using an edge finder and repeat the measurement several times for consistency.

After finding the center, I subtract the 1" from x and y to bring the offset down to the bottom left corner of the part. This becomes the offset entered into the machine.

When it's done, the part shows that the offset was off, particularly the chamfering as one or more edges have a larger chamfer than the opposite edge.

I repeated this process several times by creating several of the same part and every time I have to change the work offset ever so slightly. Can anyone shed some light on why this is happening?

I am using a HAAS VF2 with a 0.2" tip / 0.5" shank edge finder. The vise, table, and machined part (top operations) all measure and check out fine with an indicator and caliper. End mill is a 1/4" end mill, and chamfer bit is a 0.5" shank 45 deg bit.

[djr76]

Finding the center of the hole with a dial test indicator should be more accurate then the edge finder, then make your offsets from the hole. Did you mill fresh steps on your jaws before you started this job? Did you measure from the hole quadrants to the edge of the part and those numbers are right?

this is what I use to sweep a hole to find center

[HuFlungDung]

Is this a square part with a square through-hole in the center? Exactly what orientation are you using to locate the part in the soft jaws? Something like a V shaped cut into the soft jaws to locate the part in 'diamond' orientation?

Are you facing the flip side before chamfering? If the part is not exactly level, this can have an exaggerated effect on the appearance of the chamfer widths. If the movable jaw of the vise is not exactly repeatable in position, it may lift the pocket and make it impossible to actually level the part when it is flipped and faced.

I prefer to use parallels in critical flip over applications because this makes it possible to test how the part has seated: both parallels must be tight. It is possible to use a combination of parallels with soft jaws, using the profile in the jaws to locate the part in X and Y, but mill the jaws overdepth so that two parallels will hold the part slightly above the bottom of the jaw pockets.

[momospeedracer]

Originally Posted by HuFlungDung Is this a square part with a square through-hole in the center? Exactly what orientation are you using to locate the part in the soft jaws? Something like a V shaped cut into the soft jaws to locate the part in 'diamond' orientation?

The part has a fillet in the corner which is also milled on the jaws. This allows it to self center itself everytime the part is clamped.

Originally Posted by HuFlungDung Are you facing the flip side before chamfering? If the part is not exactly level, this can have an exaggerated effect on the appearance of the chamfer widths. If the movable jaw of the vise is not exactly repeatable in position, it may lift the pocket and make it impossible to actually level the part when it is flipped and faced.

Yes, the flip side is faced before chamfering.

Originally Posted by HuFlungDung I prefer to use parallels in critical flip over applications because this makes it possible to test how the part has seated: both parallels must be tight. It is possible to use a combination of parallels with soft jaws, using the profile in the jaws to locate the part in X and Y, but mill the jaws overdepth so that two parallels will hold the part slightly above the bottom of the jaw pockets.

Not sure what you mean by parallels.. can you elaborate?

djr76 - The soft jaws are freshly milled and the clamping is consistent. I can measure the same postition with the dial indicator everytime the part is reclamped.

The part is milled accurately and the dimensions correlate with my drawing.

I'm almost certain that the offset is due to my skills in measuring the center of the hole, whether it is a square or circular hole.

I don't know if this is normal practice or not as I am new to machining, but what I had to do was to measure a datum point by either edge finder or indicator, set the offset in the machine and run a part. If the part comes out visually symmetrical on the chamfer, adjust the offset manually by a few thousands of an inch and run again. Rinse and repeat the last line.

Of course this would only work for chamfers (for me at least) as anything more critical would require a more precise alignment.

[djr76]

Can we have pictures of both setups, Im curious to how rigid your second operation is. What Hu is referring to as parallels, using a set of parallels instead of milled step jaws to insure there is no jaw lift of the vise. With Parallels, you can tap the top of the part with a soft face hammer to seat the part to the parallels to insure its sitting flat. Using soft jaws with milled flats, if the steps are milled above the movable jaw plate or near to top of the movable jaw plate, it can have a tendency to lift the jaw when the part is clamped throwing the top plane off.

these are parallels if you are not familiar

[Boots]

If you are putting these parts in a standard Machinist vise then be advised that if you tighten your vise more than 45 foot lbs. (even on a new vise) then you are probably pushing the solid jaw back on the top putting your part on an angle. I have machined many parts using several vises at the same time. I discovered this anomily many years ago. You would think the vises are strong enough to take a lot of force on clamping but they are not. Put an indicator on the back of the solid jaw and tighten like you normally do and see if the indicator moves. You'll be supprised to find it moves before it gets to 50 foot lbs. So you need to use a Torque wrench to be consistant. And you may have also the problems mentioned by others. I just wanted to mention this as it will have an affect on the accuracy of your part.

[Geof]

Originally Posted by momospeedracer ....I'm almost certain that the offset is due to my skills in measuring the center of the hole, whether it is a square or circular hole...

Practice with something for which you do know the offset coordinates.

Clamp a piece of stock in the vise, face the top and either interpolate a round hole or mill a square hole.

Do not remove the piece! Make a record of the offset coordinates that were used for this hole and delete them from the machine.

Now use your edge finder or dial and re-find the offset coordinates; you know what they are and any discrepancy is due to your technique.

If you are generating a discrepancy now you play around until you find out what you are not doing correctly.

[mark c]

I noticed you said the BOTTOM left corner. Do you mean the left front corner. If so, you may find it better to change that to the left rear corner. If your part varies in size in the Y direction your Y zero will also vary if using the front of the part. Using the rear (fixed jaw) wlii get you closer because the rear jaw is constant

HTH
Mark