New To The CNC Machining Trade

[Pmp Audio]

Hi Guys,

I have been tiring to make a part that is two sided but when I flip it to mill the second side the top cuts doesn’t line up with the bottom. I’ve tried many things and have been un successful so far.


Basically I’m using 1X1 inch 6061 bar stock what I’ve done is programmed the part form the center and mill the bottom cuts first. After the bottom is milled the finished demission’s are .760 inch basically when I flip the part and clamp it in the vise the Y axis is off. I can’t clamp the part by the un milled area because there are OD cuts for the top half, Is there an easy way to set this job up?

[LeeWay]

You can use longer stock. Use a foot long bar if you need several of these parts. That way you can always clamp to the same faces. You can then either use the mill to cutoff the part or hacksaw/bandsaw.

[Pmp Audio]

Thanks for your reply,
I’ve tried that two problems that developed 1, the parts are joined by .100 and the length of stock the martial bends and flexes. 2, Also the stock tolerance is different from batch to batch so would one have to redraw the part to each lot of bar stock? The part I’m trying to make is a high tolerance part. Could I be over thinking this?

[LeeWay]

If you have lots of them to do, you could make a negative of the part and an initial blank on the same jig. Then you could mill one first cut and a finish cut at a time. You could make threaded holes in the sides of the negatives and lock the parts in place with nylon tipped screws. I'm no pro at it either. I have managed to make a bunch of different hold down solutions for my main parts I cut. They vary widely as do the different parts and materials. Maybe some of the real experts will chime in soon.
If you can take a picture or two of the part and perhaps your setup, tat would really help.

[Pmp Audio]

Hi LeeWay,

That’s an option for sure. I have been thinking about buying a bunch of stock and machine my own vise jaws fixtures exedra. Ok dumb question, would you mill all the first OP cuts then fixture the parts there after? I do have 3d models and 2d drawings do I post them here on the site or email them to you?

[HuFlungDung]

If I understand this situation correctly, the problem stems from an inaccurate reference surface. Bar stock is never truly square, parallel or straight, unless you pay extra for those features. Extruded square often has a belly to it, and it can tilt in the vise.

Depending on the precision you need, you might get away with marking one side as reference against the fixed jaw of the vise. Then, don't flip the part, rotate it so that the marked side stays against the back jaw. This will require reprogramming the operations on the second side because left and right have now been reversed.

Even doing it that way may result in a slight mismatch of features on opposing sides, because of the way that jaw/work tilt can creep in.

The best way, if you can spare the material, is to face at least one side of the stock so that it will sit reliably against the fixed jaw of the vise. Use two parallels under the stock so that you can test for proper seating of the part. Both parallels should be tight when the stock is tapped down with a dead blow hammer.

[LeeWay]

It sounded to me like his reference surface was getting milled away.
I have played with Cut 3D and the way you flip the part on it is just as described by HFD.
On the few things I did do, I had to use tabs and large material in order to keep all my reference surfaces. When completed, I would just pop those tabs off and was left with a nice 3D part and plenty of scrap for the bucket. This is not bad for one offs, but not very green for multiple parts. It would increase the cost per part quite a bit unnecessarily.

I use a negative space type thing in my router for my plastic parts. I used the same drawing, but different Gcode to make the pocket as well as the pattern I use to hand cut the plastic and round the edges over. Then it goes in the CNC and gets all the slots and dado's cut. I have some uncut areas on my parts, so it was easy enough for me to use some small toggle clamps as hold downs.

You could even use a vacuum type setup for this type thing if done correctly
Many different ways to do it. Some easier than others. Part numbers need to be taken into account as well.

You can post your drawings on here using the manage attachments feature below. Your expected part numbers would help too.

[Pmp Audio]

Hi HuFlungDung,
Hummmm, thought about that but haven't tried it yet. I'll attach a thumbnail of the part to the thread. The biggest thing is once I mill the bottom and flip/rotate it the only area left to clamp is now .760 inch .240 difference form the starting demission of 1 inch.

Thanks,
Eric

[HuFlungDung]

Against the black background, I cannot make much of that thumbnail to make any recommendations.

[Pmp Audio]

Hi HuFlungDung,

Here are a couple of new pictures. Should be able to see detail better.
Thanks,
Eric

[HuFlungDung]

That is fairly tricky, isn't it

For best appearance, I think I would mill the part with the legs facing up first. I would use a piece of stock that is high enough that I could grip a sacrificial sliver along the bottom (say 1/8 to 3/16 thickness) in the vise. Mill all the features that you can in this initial setup. I assume you are using some sort of chamfer mill to mill the sloped dovetails. This will give you completely finished faces where they bulge out in arc form, instead of trying to match those up by machining halfway and then flipping.

Then, machine a spacer for the part. This spacer should be of such dimensions that it is a close fit in the groove through the part, and has a small circular boss on top to engage the round hole that you have already milled in the part.

If you are in mass production mode, you should be able to make this spacer long enough to contain 3 or 4 circular bosses, so that you can mount 3 or 4 parts for the secondary operation.

Of course, this spacer is a precision part, and you will need to have one of its ends faced to serve as a datum against an end stop on the vise jaw.

Set the half finished pieces up so they straddle the spacer and engage the boss. Then clamp the part in the vise across the flats of the legs. The spacer then serves the purpose of preventing the part from collapsing from the pressure of the vise.

Use a dial indicator in the spindle to sweep the holes where the engage the boss on the spacer. This assures a correct initial setup. In your CAM, create a new program assuming the part position is centered with the XY datum on the hole.

Facemill the top of all the parts, removing the sacrificial material, and then finish the counterbore in the part, above the locating boss. Mill the chamfer dovetail as the final op.

[LeeWay]

On the second read, I agree with HFD. This would be a good way to handle it. It would still be a bit tricky and require some good setup. I would mill the bottom first, however I would mill out the hole completely in the first op. Then you could use this to setup the second cut precisely in the center.

A cheap center finder would really help you out here. It sound like because your vise jaws changed position after the initial cut, you were not able to get exact center on the second.

That said, if this clip isn't really load bearing, this part looks like a good candidate for injection molding in plastic. Small oddball shapes like this are not all that costly in quantities of 500 and more. You have to make it worth the mold cost initially, so the more you need, the cheaper they become. Some plastics are incredibly strong especially for small parts.