Work Holding And Order Of Operation

[JimDawson]

Sometimes even a very simple part presents some interesting challenges in work holding.

I needed to make a small spacer to mount a heat sink for an 80 Watt LED. It’s 6061 aluminum, U-shaped, and 0.300 thick. Being a U-shape hanging on to it is a bit of a challenge, and I had to machine all of the surfaces. Once the U is cut out, it can’t really be held in a vice because it will squish. On most projects I machine the whole project in my head before I ever make a chip. So here’s what I came up with.

The finished part



I added a bar on the open end of the U to stabilize it in subsequent operations. The roughed out blank. Made of 0.500 thick material that I had on the shelf, and cut 0.300 deep with a 3/8, 2 flute end mill



Finishing the inside with a 1/8 end mill because I needed corner clearance.



Next I cut out the blank on the band saw then mounted it upside down in the vice to face to 0.300 thick



After cutting down to 0.300. The bar on the end is keeping if from squishing in the vice.



Now it’s time to cut off the bar and trim to length, so over to the band saw then back to the mill.



Trimming to length. I left it hanging out of the vice a bit so I could get a mic on it to measure it.



The exploded view



and the kind of assembled view, the screw holes have not been tapped in the heat sink yet.

 

[Ripthorn]

Very nice. Sometimes the best information one can give is the stuff that seems perhaps unglamorous. However, for those of us who are newer to this, learning how the experienced guys go through the process is much more valuable than discussing some of the other more frequent topics. I wish there were more threads like this, as sometimes I find myself trying to go through it in my head as well, but coming from a woodworking background, there are considerations that are not automatic for me.

 

[brino]

Jim,

Thanks for the great, thorough explanation/documentation of both your project and thought process.
I know it takes much effort to stop, photograph, transfer/upload, and then finally put some words around them.

It is very much appreciated!
-brino

 

[kvt]

Thanks, First the head, Then put it on paper, or in my case a cardboard box or something, Then work on it. But for some reason it does not turn out as nice as yours. What my head thinks, and what actually comes out of the lathe and mill do not always match.

 

[RJSakowski]

Thanks, Jim.
Work holding is probably the most important and least thought-through process of the machining operation. Quite often, leaving a "handle" on the part is the easiest way to attack the problem.
BTW, What is the 80 watt LED? That is some hunk of power!

 

[JimDawson]

BTW, What is the 80 watt LED? That is some hunk of power!

It's a UV LED for adhesive curing. 20 Amps at about 4.1 volts. You would not want to look at it, would instantly fry your eyes. In use it will be 100% shielded to protect the machine operator and anybody else in the area.

 

[RJSakowski]

It's a UV LED for adhesive curing. 20 Amps at about 4.1 volts. You would not want to look at it, would instantly fry your eyes. In use it will be 100% shielded to protect the machine operator and anybody else in the area.

A few years ago, I developeda product which required bonding PEEK to glass. We used UV curing adhesive from LocTite and UV pointers for curing. Their output was about 200 mw and curing only took a few seconds. I can't imagine what 80 watts would do.

 

[JimDawson]

Another example of a multi-step machining operation. The goal of this thread is to show the thought process that goes into making the part while minimizing any errors that can creep into the process, as well as a proceeding in a logical order of operation to minimize setup and tool changes.

I am helping another member, Alloy, retrofit his Shizouka AN-S CNC mill http://www.hobby-machinist.com/threads/shizouka-an-s-build.33868/

For system compatibility and ease of control we decided to power the tool changer with a stepper motor rather than the Geneva drive system that it had originally. I designed a 16:1, double reduction, inline gearbox that will fit in almost the same footprint as the original system.

The concept:



The layout for machining operations. The material is a chunk of 6061 aluminum 19 x 6 x 0.75 .
Turns out I only needed about 17 inches. The part drawing is overlaid on a drawing of my mill table so I can get the bolt hole layout to align with the T-slots.

Since I do most of my machining in the lower left quadrant ( -X, -Y) ( it's a long story), 0,0 is at the upper right corner of the work. The dimensions are to 4 decimal places on the drawing only because this is what I have the CAD program set to, the actual positioning on the table is done with a tape measure and a scale. Not terribly accurate, nor does it need to be for this part of the process.

This drawing shows the upper and lower gear case halves laid out on the work piece. The dimensions on the drawing are to position the work on the table, and to pre-stage the t-nuts under the work. I won't be able to get to some of them once the work is bolted to the table.



First the spindle is set to the center of the middle T-slot, Y = -3.000 in this case, working 0,0 will be set after the work is bolted to the table. The work is positioned and clamped to the table with normal clamps until the bolt holes are drilled. X zero is set once the work is clamped down. This allows the bolt holes to be drilled through the work and the 3/4 inch MDF backer board. Then go back and C-sink the bolt holes for 1/2'', flat head cap screws, C-sink deep enough that the screw heads won't be hit during the facing operation. The Sharpie marks on the table are where the T-nuts are positioned under the work. Once the work is bolted down and the clamps are removed, then the working 0,0 is reset at the upper right corner of the work. This position will not change for the duration of the process.



Once the working surface is flat, then time to drill (and tap as needed) all of the holes needed. First center drill all of the holes, then go back and I'm working with a CNC machine here, but everything I am doing also applies to a manual machine except that the process and part would change just a bit and I would make use of a boring head quite a bit more. With a manual machine I would also just round off the end on a rotary table as the last step in the process, rather than profiling it as I did here, but the rest of the process would remain pretty much the same. The outside profile is not a critical dimension so anything close is fine. The critical dimensions here are the bearing bores, and the axial spacing for the gears.



Once the holes were drilled, now is time to change over to the 1/2 finishing rougher end mill (now there's an oxymoron)



The internal gear housings have been pocketed, and the lower output bearing bore was done with the boring head. Then work was bolted down through the axial holes to the pre-staged T-nuts. The work was never free on the table, the flat head cap screws were then removed for the next operation.



The rough outside profile is complete, about 0.050 oversize. All of the internal work has been done on both of the gear housings, except the 7/16 axle hole, this will be the last operation.




Once rough profile was done, then I removed the upper gear case from the table and flipped it over onto the bottom gear case. I used some flat head screws to align the two parts and hold them together while drilled and reamed the dowel pin holes. Now these parts are married and can't move. Then I went back and C-bored for the socked head cap screws and bolted the halves together. At this point I still have not un-bolted the lower gear case from the table so zero position has not changed.



Now it's time to cut the motor aligning pocket. Because I have not moved the lower gear case, this pocket will be aligned with the output bearing bore. The center hole there is just clearance, not a critical dimension. The motor pocket is a critical dimension, and it is 0.001 larger than the flange on the motor.



Finish profiling the work, because the parts are bolted and dowel pinned, it will look like it was supposed to be, rather than just happening that way.



There is still one operation left, and that is the axle hole for the intermediate gear set, that is the 3/8 hole in just to left of center.

I was my intention to drill and ream to 7/16, but I found that the drill bit had walked a bit and the hole was about 0.005 off of where I wanted it. I tried to find an under size 7/16 end mill in my stash, but no luck. I would have used a boring head to re-locate the center on a manual machine, but in this case it was just as easy to pocket the hole. Once that was complete, I unbolted the top gear case, and need to pocket the axle hole in the bottom gear case. Only the 3/8 bolt was removed after the clamp was installed on the back, using one of the pre-staged T-nuts.




The operations on the gear case are complete, now I can unbolt the lower gear case from the table.

The parts. There is still some work to be done on the gears.



The output gear rides in a bearing in the lower gear case so the hub had the be turned to fit. The bore from the factory is concentric with the OD of the gear, so I turned and threaded a stub arbor to hold the gear while turning the hub OD. I didn't have a tool in a holder that I could reach past the OD of the gear with, so I just grabbed a boring bar that was already in a holder to turn the OD. I just turned the spindle in reverse for this operation.

Kind of an exploded view of the setup.



Pocketing the other side of the gear for the lower motor shaft bearing, This gear will be turning at 1/16 the RPM of the motor shaft. Setting up the bearings like this insures things won't walk around inside the gear case.

I again centered up on the bore, and completed the operation. Again, this could have been done with a boring head.





And there it is!



And kind of in place, need to relocate the rear mount a half inch to get every thing to fit and rotate it into position.

 

[JimDawson]

Sometimes a production fixture is required to efficiently machine parts. In this case I need to run about 100 piece orders, and these will recurring about every 6 months or so. Cost of the fixture is a consideration and given that these are short runs I didn't want to spend too much time or money on the fixture, so I chose to build it from MDF. If this were a high production part or required coolant for machining, then I might have chosen aluminum or steel for the fixture material. In this case the part is UHMW, which is like cutting thick grease, so no cutting fluid required.

A lot of thought should go into fixture design. It needs to be able to securely and accurately locate and hold the work for the machining operation, and needs to be easy to load and unload with minimal effort. In this case, the location tolerance is +/- 0.010 so extreme accuracy is not required. It also needs chip clearance to keep chips from building up in the corners and locating surfaces.

So here is what I came up with for this operation. I cut out the pieces on the router. I added two 5/8 dowel pin holes for alignment during assembly. If I had been thinking, I would have positioned the dowel pins to locate the fixture in the T-slots on the mill, that way I wouldn't have to indicate it in. I thought about this as soon as I put the fixture on the mill, oh well, next time.



A little wood glue to make it solid block when assembled, keeping the glue away from the locating surfaces.



And all screwed together. The screws are 3 inches long and go through all of the pieces. I normally use deck screws in MDF.



When designing the fixture you have to take the cutting forces into consideration. In this case due to the cutter rotation the primary force is left to right, so the locating stop needs to be on the right end. There is also some vertical force, with the cutter trying to pull the part up due to the spiral angle on the cutter (think about drilling through an unsecured workpiece). The larger the cutter, the more pronounced the cutting forces are. So I added an anti-lift plate to the top. I am not happy with the clamping system that I am using right now, so I am going to rebuild it. It holds fine, but even with the rubber pads on the bolts, it is still leaving a mark on the surface. Note that the cutter parking position is well away from the working area so the spindle motor does not have to be turned off during load/unload operation.



This is the end mill, 2 inch dia, 3/4 shank.



Here is an overview




The chip clearance is important, you can't allow a corner where chips can build up. In this case it's pretty easy because the all of the corners on the part are all rounded over, so no clearance is required except at the end. If the part had square corners then I would have provided chip relief areas in any location where a part corner would meet the fixture. A quick shot of air and the chips are cleared out.



The toggle clamps work well, but the pressure pads are not working well. They were OK for the dozen ''first article'' parts, but will be corrected for the rest of the run.




And the clamps open. plenty of room to load/unload.



And in action



I'll post pictures of the modified clamps when I get them done.
.
.