Workholding Suggestions Please

[UKRobotics]

Hi All,

We'll i've slowly been progressing from little toy routers and mills machining plastic upto a big industrial steel munching bridgeport. I've taken time to learn cad, and cam to a level where I can do something useful with it and what a steep learning curve that was.

Now I have a new problem and I'd be every so greatful for some advice from seasoned machinests.

In the good old days of the 'toy' machines i was only cutting plastics usually quite thin with equally small cutters. Typicallly I would hold a part in a vice just so it was firm but not too tight so as to warp the material and use double sided tape underneath to hold everything in place. It was cheap, simple and effective (if a little crude) and even worked on the occasional bit of ali so long as i used a small diameter cutter with low feeds and pass depths.

Now i'm in a whole new world of considerably faster feeds/speeds/ bigger cutters and chunkier metal. Having learnt some cad/cam basics and thinking that was the hardest part out the way i'm now struggling with what i thought would be the simplest thing - holding the workpiece down to the table!

So i'm trying to machine out this simple part from a piece of ali that is the same thickness as the part needs to be in the thickest point (10mm) and theres only about 14mm spare material round the outside. (i'm trying to make this from offcuts rather than spending out money on new stock!)




I put the material in the vice and made a toolpath with tabs on the outer contour, the intention being that there would be enouhh material to hold it in place to finish the cut and then it would be a small job to finish off with a hacksaw. However it didnt really work as planned and when all the tabs where cut the part slipped out the jaws and i had to abort.

So given the part and the circumstances i'd be really greatful for some tips on good workholding technique that would work in this situation.

A technique i have used a few times is clamping a block of wood into the vice , drillling some holes in the ali material to be machiend by hand and then screwing the ali plate to the wood. again its crude and you do tend to get a bit of movement/vibration but it has got me by but i'd really like to learn some better options even if it means buygin some special kit.

I had an idea about maybe getting a big thick ali/steel plate and drlling/tapping a few hundred M6 holes in it and then useing that to screw clamps into. Not sure if it would be as good as I'd hope tho. i could see the threadded holes gettign clogged with swarf in no time.

[M250cnc]

Dom i come from an era before CNC so i am used to working that way.

You are trying to do the whole part in one set up and that is why you are failing.

Leaving tabs can work but you need substantial material to hold the part in a vice and not crush the scrap area.

Looking at your part i would do it in two op's

You need various parallels for the vice to allow for the material to come near the top of the jaws.

Unless you are machining wood you cannot use wood to fix a piece of metal to it and then machine the metal.

So fix the billet in your vice with the billet protruding 6mm above the jaws, this is assuming the raised boss/island is 5mm high.

Machine every thing except the outer profile.

Then clamp in the jaws using the boss/island in the middle.

Find and locate one of the holes to a ref position and machine the outside.

Phil

[Geof]

The suggestion above is probably the best way to go about it.

Generally the best approach, on just about any job, is to figure out which dimensions are important and which are not. In this case the hole spacings and the size of the rectangular protrusion are probably important, the larger perimeter if probably not as important. So grip the stock, on parallels as suggested or make yourself some step jaws, and machine all the important features in this setup. Then flip it and finish off the less important features. To make it easier to find the work zero reference after flipping the part choose a location that is created during the first machining. By this I mean do not choose a corner of the original stock choose, for instance, the central large hole as the work zero for the both operations. It is a trivial matter once the pasrt is flipped to dial into this hole very accurately to get good registration between the first and second operations. Choosing a central feature such as this also simplifies programming when it is done by hand because the code is symmetric about this point.

[UKRobotics]

Thanks Phil and Geof, I think i understand where you are coming from and see how that would work.

The only bit i'm unsure about is how to set the work zero reference. Lets take your example of using the centre hole as the origin. If I do that, when it comes to machining the first operation it'll be a bit of guesswork to position the part on the material where as normally i'd just zero on the bottom left corner.

Then when it comes to turning over the part and doing the second operation how do I go about accurately zeroing off that position? The slot drill is smaller than the hole so I cant just feed it in and zero knowing it will be central? So how is this done should i zero to the edge of the centre hole rather than the middle ? and even then how would I get that measurement accurate?

[M250cnc]

Not really, there are so many ways to do this.

Instead of zeroing the bottom corner you set an offset that brings it to the centre of the billet. But you don't even have to do that, you could leave it at 0 0 then put an offset for any hole you reference in op two.

To find the center of a hole you can use a DTI or a probe, then you set the DRO' s to match the part dimensions.

Phil

Sent from my HTC Desire using Tapatalk

[Geof]

It is just as easy to find the center as it is to find the corner. Actually you find the corner first then move half the stock dimensions in X and Y and you are at the center,

When the part is flipped you find the center of the hole by mounting a dial test indicator (DTI) in the spindle with the probe against the side of the hole. Rotate the spindle and adjust the X and Y position until the DTI shows no deflection and you are on center.

Or use a Coaxial Indicator:

YouTube - Dial co-axial Centering Alignment Indicator

[M250cnc]

Originally Posted by Geof It is just as easy to find the center as it is to find the corner. Actually you find the corner first then move half the stock dimensions in X and Y and you are at the center, When the part is flipped you find the center of the hole by mounting a dial test indicator (DTI) in the spindle with the probe against the side of the hole. Rotate the spindle and adjust the X and Y position until the DTI shows no deflection and you are on center. Or use a Coaxial Indicator: YouTube - Dial co-axial Centering Alignment Indicator

Is there an echo in here ?

Sent from my HTC Desire using Tapatalk

[Geof]

Originally Posted by M250cnc Is there an echo in here ? Sent from my HTC Desire using Tapatalk

Yes, I started on my post and was interrupted. But at least we echoed not clashed like sometimes happens with advice from two sources.

[fizzissist]

Originally Posted by UKRobotics Thanks Phil and Geof, I think i understand where you are coming from and see how that would work. The only bit i'm unsure about is how to set the work zero reference. Lets take your example of using the centre hole as the origin. If I do that, when it comes to machining the first operation it'll be a bit of guesswork to position the part on the material where as normally i'd just zero on the bottom left corner. Then when it comes to turning over the part and doing the second operation how do I go about accurately zeroing off that position? The slot drill is smaller than the hole so I cant just feed it in and zero knowing it will be central? So how is this done should i zero to the edge of the centre hole rather than the middle ? and even then how would I get that measurement accurate?

Another method that is good to keep in your repertoire is clamping below what will be the finished part...that is, the blank is thicker than the finished part by some nominal amount, and you clamp on that region, with a small relief. When the first operation is completed, which includes finish milling the outer contour, you flip the part over and face mill that clamping region down to the finish thickness.

This means wasting some material, but allows you to maintain perfect concentricity or dimensional relationships by doing everything in one clamping.

There's a clamping system called Talon Grips, you can see here:
TalonGrip Systems, Inc.

I have found them invaluable for some jobs, on aluminum and SS. You'll only sacrifice a tad over .06" for the facing op. (I took a kiss cut off the top of the jaws when first installed to guarantee the clamping surface was dead flat relative to the machine table, and that was it). They work quite nicely in a regular Kurt vise.

If you set up a second vise, one for these and one for the finish face-to-thickness and cut & paste the two ops together, it'll make production faster and easier.....and there's more time for coffee after you've deburred the last part while running the cycle.

....And that's what it's all about, right?

[Geof]

Originally Posted by fizzissist ....and there's more time for coffee after you've deburred the last part while running the cycle. ....And that's what it's all about, right?

And if you get dovetail and/or lollipop cutters you can have the machine do all the deburring as well making even more coffee time available.

Not really worth it for small quantities but a real timesaver for production work.

[fizzissist]

Originally Posted by Geof And if you get dovetail and/or lollipop cutters you can have the machine do all the deburring as well making even more coffee time available. Not really worth it for small quantities but a real timesaver for production work.

...Hmmm....Hadn't thought of doing the back-burring with a dovetail....GREAT idea, Geof!!

That'll justify that new 10-cup I've been looking at..