[4]

Steady Rest

[3]
[10] Like what you see?
Click here to donate to this forum and upgrade your account!

JimDawson

Global Moderator
Staff member
H-M Platinum Supporter ($50)
Joined
Feb 8, 2014
Messages
7,837
My lathe did not come with a steady rest and for the first time in over 20 years I actually need one for a project. I have to drill a 1 inch hole about 20 inches deep through a UHMW rod about 3.5 inches dia. Way too much stick out to do it unsupported. When I get to that project I'll post showing how I did it.

I looked on line for a steady rest that might fit my lathe, but what I found were all much too small to handle anything close to 3.5 inches. I can put 6 inch diameter over my cross slide, so you would think that a little bigger hole would be available in a steady rest.

OK, so sit down and design a steady rest that will do what I want. This one will handle a max of 4.5 inches. The design has changed slightly from this drawing. There will be bearings added to the fingers. But I will also make a set of brass fingers with no bearings. The clamp bolt design has also changed to a swing away clamp.

upload_2016-4-19_21-3-57.png

I spent most of the day digging the top part out of a chunk of 4x7.5x1 6061.

I bolted the part down to a MDF spoil board with one 1/2 inch bolt to a T-nut under. Then drilled and tapped for 1/4-20 right into the MDF just to prevent any possible rotation when machining. I started by pocketing the lightning relief, not really to make it lighter, but just to make it look more professional.

1/4 inch, 2 flute, solid carbide router bit. 2400 rpm, 10 IPM, 50/50 mix of kerosene and WD-40 for cutting fluid. I limited the depth of cut to 0.063 because the setup was not the most robust. I would have rather had more bolts in there but no place to put them.

upload_2016-4-19_21-18-16.png

Putting the radius in the bottom of the pockets, just to make it look nice.

upload_2016-4-19_21-20-11.png

Profiling the outside surfaces. This is where it gets a little dicey, I wasn't sure how things were going to react when the piece that is bolted down with the 1/2 inch bolt gets cut loose from the actual part. There is not much holding things down. I went outside until this part of operation completed to get a wall between me and the machine, I didn't want to get hit with flying carbide. :cautious: As it turned out, everything was well behaved, and went exactly as planned.

upload_2016-4-19_21-29-12.png

And the back side of the top is complete. That little flat on the hinge radius was not designed in, I really needed 4.125 wide material but only had 4 inch. No problem, it will work fine, and that part is hidden anyway.:rolleyes:

upload_2016-4-19_21-30-34.png

Now for the other side. First I machined a 0.250 deep pocket into the MDF with the same profile as the part. This allowed a press (OK, hammer;)) fit that captured the part and holds it securely. As you can see, this spoil board has been used for a few other projects. Just about past it's useful life.

upload_2016-4-19_21-33-42.png

Pocketing the front side. The part is held down by one 1/4-20 cap screw threaded into the MDF, it really can't go anywhere, and I probably didn't need the cap screw, but a little extra insurance doesn't hurt.

upload_2016-4-19_21-38-53.png

And the (almost) finished part. I have to do the clearance and slot for the clamp bolt, but that will be after I get the rest of the parts done and put the vice back on.

upload_2016-4-19_21-42-6.png


Somewhere in that 8x10x1 chunk of aluminum is the bottom, I'll dig around in there tomorrow and see if I can find it.;)

upload_2016-4-19_21-43-48.png
 

Black13

Active Member
Registered
Joined
Jan 16, 2015
Messages
26
Looks great!
Can't wait to see the finished product, keep the pics coming.
 
D

Deleted member 34477

Guest - Please Register!
Guest - Please Register!
Awesome work Jim, keep us updated.
 

T Bredehoft

Active User
H-M Supporter - Gold Member ($25)
Joined
Dec 27, 2014
Messages
3,054
If I had CNC on my mill I'd cheat a lot. I can't see a tool changer on a MP25, though.
 

JimDawson

Global Moderator
Staff member
H-M Platinum Supporter ($50)
Joined
Feb 8, 2014
Messages
7,837
Yesterday I got the top half completed, so today is find the bottom half in that block of aluminum

upload_2016-4-20_19-59-52.png

So here it is all bolted down on a sort of fresh spoil board. The bottom is in there, just need to find it.:)
upload_2016-4-20_20-2-10.png

The pocketing is complete on one side. I started with the pockets and will do the other operations while it's bolted down solid. Then do the cut off last.
upload_2016-4-20_20-4-35.png

The finishing cut on the outside profile. Note, I didn't cut out around the hex head bolt, I'm going to use that hold down in the next operations. But the outside is on size.
upload_2016-4-20_20-6-39.png


Corner rounding the outside with a 1/16 radius corner rounding end mill. Note the clearance pocket around the hex head bolt. This allowed clearance for the corner rounder. A stack of spoil boards in the lower left of the picture. It's my preference to bolt parts to the table when possible rather than use a vice. That's why they invented T-nuts and T-slots.;)

upload_2016-4-20_20-9-38.png

And ready to flip over and do the other side. The 1/4-20 button head screws are threaded into the MDF spoil board.

upload_2016-4-20_20-14-54.png

I cut a 0.250 deep pocket to locate the part for the second operation. Again a hammer fit.

upload_2016-4-20_20-16-38.png

And bolted into place. The socket head cap screw in front of the part is just to insure the spoil board doesn't pull up in the center. I used a flat head cap screw in the back to make sure I had tool holder clearance when working in that area.

upload_2016-4-20_20-19-43.png

And here are the two halves. Now I need to cut the slots for the hinge and for the clamp screw.

upload_2016-4-20_20-22-18.png


I'll get the base done tomorrow and get the slots cut. Stay tuned! :grin:

EDIT: I forgot to add that it was really exciting running a CNC machine in the middle of a thunder storm, but I wasn't about to shut it down in the middle of the work. Yeah, I'm crazy :confused:
.
.
 
Last edited:

JimDawson

Global Moderator
Staff member
H-M Platinum Supporter ($50)
Joined
Feb 8, 2014
Messages
7,837
I got a bit more done in the last 3 days, pesky customers keep wanting stuff.

Prepping to put the clamp bolt relief in the bottom side of the clamp. First I milled a pocket to locate the part and keep it from moving around. I could have done this operation in the vice, but I already had the spoil board on the table so I just used it. Only takes a few minutes to cut the pocket.

upload_2016-4-23_19-58-5.png

I located the pocket next to a bolt hole so I could clamp the part down. The part is held securely by the pocket, so only one clamp is needed.

upload_2016-4-23_19-59-50.png

And the bolt relief completed. The slot on the left side was an oops, but it will be gone in the next operation.

upload_2016-4-23_20-5-15.png

The next operation is to radius the clamp to roughly match the tailstock clamp on the left. This is required due to the shape of the lathe bed.

The radius is about 2.8 inches. I concidered a number of different ways to do this. It could be bolted to an angle plate on a face plate on the lathe, bolted to an angle plate on the rotary table, mounted on an arbor on the 4th axis rotary.

upload_2016-4-23_20-15-20.png

Or mounted in the vice and just mill the curve which is what I decided to do. I did 1/2 at a time, just flipped it over and did the other half.

upload_2016-4-23_20-23-38.png

And the finished part
upload_2016-4-23_20-24-33.png

Now to finish the base. I was going to do this operation in the vice but I found I had miss-measured :( the length in the initial design so I needed to take off 0.193 off of each end to keep the holes on center. So I used the pocket fixture technique again so I could work on the V-slot as well as the ends.

The tool bit is a 90° carbide tipped, 3/4 inch dia. router bit. Finish depth is 0.375, @ 0.015 DOC, 2400 RPM, and 10 IPM. I went pretty easy because of the width of the final cuts. In retrospect, I could have taken a bit more but I'm not in that big of a hurry.

upload_2016-4-23_21-0-48.png

And the finished part. The extra hole on the the right edge is the result of the miss-measurement mentioned above. So I moved the hole to the center of the V-slot.

upload_2016-4-23_21-3-49.png

And the assembly kind of in place. Still need to cut the hinge slot, the clamp knob slots and clearance, make the clamp knob, and drill & tap the mounting holes, and make the fingers. And do to the miss-measurement the bottom half needs to be modified at the base. so still quite a bit of work to do.

upload_2016-4-23_21-17-53.png

Stay tuned!
 

JimDawson

Global Moderator
Staff member
H-M Platinum Supporter ($50)
Joined
Feb 8, 2014
Messages
7,837
I forgot to add these pictures from yesterday.

I needed to modify the hinge end of the top part. I didn't allow enough clearance in the pocket area below the hinge in the lower piece so back to the drawing board (OK, computer) for a bit and figure out how to fix the problem. I'm not about to buy another $40 worth of aluminum to make a new bottom piece.

upload_2016-4-23_21-55-56.png

So I pocketed the spoil board to fit the part and trimmed up the end a bit. Again the pocket locates the part and allows minimal clamping.

upload_2016-4-23_21-56-32.png

And the modified part

upload_2016-4-23_21-58-42.png

Getting set up to cut the top of the base.

First check the bolt length. I use T-nuts without deformed threads in the bottom. This allows the bolt to screw through the T-nut, but you have to be mindful and not allow the bolt to screw through the T-nut and into the bottom of the T-slot. In extreme cases it would be possible to actually break out the T-slot.

upload_2016-4-23_22-9-34.png

Bolted in place. Pocketed the two reliefs that locate the bottom half. Then cut the outside profile. I went easy because it's only held with one bolt. 0.063 DOC with a 1/4 inch solid carbide router bit.

upload_2016-4-23_22-16-59.png

I checked the fit of the pockets before I tore down the setup and found it was a bit undersize. So I re-ran to pocket routine again with a tool offset to account for the undersize.
upload_2016-4-23_22-24-31.png
 

wrmiller

Chief Tinkerer
H-M Supporter - Gold Member ($25)
Joined
Mar 21, 2013
Messages
3,564
Nice work Jim. I think I know who I'll contact if I need some parts CNC'd :rolleyes: :D
 

JimDawson

Global Moderator
Staff member
H-M Platinum Supporter ($50)
Joined
Feb 8, 2014
Messages
7,837
Thanks Bill :), I hear what you're saying. ;)

These project posts are more about problem solving, order of operation, and work holding than the actual machine work being done. Hopefully the readers can take away some bit of information that will help them in the future.

If I were going to do this same project on a manual machine, the design would have been a little different and it wouldn't have been so ''swoopy" with the nice curves and lightning pockets. But just about any project I post on this forum could be done on a manual machine, having a CNC just makes it easier with less setup time. On the other hand, the CNC requires that you think through the entire process before you ever make a chip.

Consider also that about 4 years go I couldn't even spell CNC:oops:, in fact, I had the machine for about a year before I had enough guts to even use the computer for anything but a DRO and a jogged power feed. But once I overcame my unfounded fear :cautious: of this newfangled stuff it opened up a whole new world of possibilities.
 

wrmiller

Chief Tinkerer
H-M Supporter - Gold Member ($25)
Joined
Mar 21, 2013
Messages
3,564
A little tongue in cheek Jim, but I was also complimenting at the same time. I will call you if I need a run of parts or something too difficult to do on my manual. :)
 

Eddyde

Bronze
Registered
Joined
Oct 13, 2014
Messages
1,504
Jim, As usual excellent work, the extra effort you took to make it look nice as well as it will functions is the mark of a true craftsman.
 

JimDawson

Global Moderator
Staff member
H-M Platinum Supporter ($50)
Joined
Feb 8, 2014
Messages
7,837
A little tongue in cheek Jim, but I was also complimenting at the same time. I will call you if I need a run of parts or something too difficult to do on my manual. :)
I understood what you meant, and understood the compliment.:) Thank you.

Jim, As usual excellent work, the extra effort you took to make it look nice as well as it will functions is the mark of a true craftsman.
Thank you for the kind words Eddy! :encourage:

At the end of the thread, I'll go through the design errors and the machining errors and explain how I fixed them and what I could have done to prevent them.
 
Last edited:

JimDawson

Global Moderator
Staff member
H-M Platinum Supporter ($50)
Joined
Feb 8, 2014
Messages
7,837
Thank you for the kind words Tom.:tranquility:
 

sanddan

Active User
H-M Supporter - Gold Member ($25)
Joined
Jan 22, 2012
Messages
651
Just found this project, great job so far Jim!

If you were running the CNC during the thunder storm we had recently the only comment I can make is WOW. I was hiding in the house afraid to go outside. That was some storm for us Oregonians.

The use if the spoil boards is very interesting, I assume these are not just for CNC but can be used on manual machines when needed. How consistent is the thickness of the MDF board? Does this hold the part parallel to the table accurately enough for the finished part or do you do a final cleanup?

Looking forward to the next installment.
 

JimDawson

Global Moderator
Staff member
H-M Platinum Supporter ($50)
Joined
Feb 8, 2014
Messages
7,837
Thank you for the kind words.

Yeah, that was quite a storm. But by counting the seconds between the flash and the thunder, the closest strike to me was about 7KM. (it's easier to calculate in metric units, ~1100 M per second). Most of it was cloud to cloud.

MDF is pretty consistent. If there is a question you can always take a cut on the surface and make sure it's flat. I have found that it holds lateral position very well. There is no reason you couldn't use it with a manual machine as a spoil board or fixturing. On the CNC it is really nice because you can cut a mirrored pocket and flip the part over and work on the other side with a high degree of confidence that the part is located correctly. More accurate than edge finding. I find that MDF is a pretty versatile material in the shop, and it's cheap. I normally buy 3/4 inch.

If I needed to hold better than 0.001, MDF would not be my first choice. In that case I would use aluminum or steel and surface it in place.
 

JimDawson

Global Moderator
Staff member
H-M Platinum Supporter ($50)
Joined
Feb 8, 2014
Messages
7,837
I got a bit more work done

First order of business was to fix my stupid measuring mistake. If you look at the picture, the bottom hangs over the base by 0.193 on each side but worse than that, it is also of center, so 0.013 off of one side and the rest of of the other. The worst part was that it would not fit between the carriage rails.
Double check the measurements before making chips, it will save a lot of work.:cussing:
upload_2016-4-25_22-41-50.png


So back in the mill and make the modifications and try to make it look like it was supposed to be that way:rolleyes:
upload_2016-4-25_22-43-5.png

OK it fits now and clears everything, but it looks like crap. :mad: This will haunt me every time I use this tool.

upload_2016-4-25_22-48-28.png

OK enough whining.:faint:

On to the fingers.

First create a work surface. I was going to bolt down an aluminum plate the the table to mount the work on, but I found this chunk of 6'' aluminum channel in the miscellaneous stock rack, and I needed the vice for the next operations anyway. Had to remove the rear jaw to get it in there. Then of course when you tighten up on a piece of channel it wants to bow up in the center a bit, so a light facing cut to flatten it out.

upload_2016-4-25_23-6-54.png

Then drill & tap the mounting holes. These will be used later.
upload_2016-4-25_23-8-13.png

The work piece is 1/2 1018 cold rolled steel. I had to clamp the channel down also because it tried to pull up on me when I was tapping. The pilot holes are also drilled where the pocket start, much easier on the end mill. Even center cutting end mills don't really like plunge cutting. That's why drill bits were invented.;) For the moment the work is just clamped to the aluminum

upload_2016-4-25_23-16-49.png

OK, the slots are cut and in the middle of the chamfering operation. I used a 1/4 inch, solid carbide router bit to do the slots. 2400 RPM, 10 IPM, 0.063 DOC. Made the slots 0.260 wide for bolt clearance.

upload_2016-4-25_23-21-48.png

Here is the work screwed down. And starting the outside profile operation. Remember what I said earlier about end mills not liking plunge cutting? Well I should have drilled pilot holes because on the next pass after this picture the router bit shattered. It was plunging too fast. :( I guess I got pretty good life out of that one anyway, it had done all of the work on this entire project up to this point and a few others. Router bits are not quite as robust as end mills, the web is a bit thinner. But they cut great, are razor sharp, and available on a Saturday afternoon at your local big box store.

upload_2016-4-25_23-30-49.png

The only sharp 1/4 inch end mill that I could fine was a HF 4 flute. It did the job but it won't run as fast as the carbide so I had to slow the feed down also. So about 90 minutes to cut these 3 pieces out, including the tool change.

upload_2016-4-25_23-40-16.png

and the near finished parts with the bearing mount holes drilled, tapped, and reamed to depth.

upload_2016-4-25_23-41-46.png

Now for the bearing clearance. Just lined them up in the vice, squared them up, and away we go:) Note the emory cloth between the movable jaw and the parts, grit side to the parts, that insures that nothing is going to move.

upload_2016-4-25_23-47-52.png

And the slots complete. 3/16 cobalt, 2 flute. 10IPM 0.035 DOC, 1800 RPM. The slots are 0.520 deep to clear the 0.500 bearing. I would have used 0.750 bearings, but I had 0.500 in stock.
upload_2016-4-25_23-46-18.png

And the completed fingers

upload_2016-4-25_23-52-46.png

This will handle a full 4.5 diameter part in the lathe and go as small as about 1/8 inch.

upload_2016-4-25_23-54-35.png

A little teaser for the next operations ;) Stay tuned!............

upload_2016-4-25_23-57-29.png
 

JimDawson

Global Moderator
Staff member
H-M Platinum Supporter ($50)
Joined
Feb 8, 2014
Messages
7,837
The next operation is to pocket out the clearance for the clamp handle. I didn't want the clamp to protrude out like below

upload_2016-4-26_8-6-30.png

So it gets buried back into the top. This is the one exception to plunging with an end mill. If you take small bites, less than about 20% of the end mill diameter, an end mill will plunge just fine. Using a 3/4 inch x 4 inch end mill and 0.063 step over, it took about 5 minutes to rough out the shape. Then go in and finish the profile to final dimension.

The following pictures are a little strange, I hit some button on my camera and managed to set it for using the flash all the time. For some reason they came out with a red tint, and with the flash the shutter speed is so fast that it ''stops'' the spindle. That is turning about 1200 RPM in this picture.

upload_2016-4-26_8-7-56.png

Now for the bolt slot. A quick setup with a level. I leveled my mill so I could use a level for setups. This only needs to be close, it's just for bolt clearance. It doesn't need to be held to 4 decimal places, no point in chasing zeros when you don't need to. :confused: If a part needs to be held to 0.0001 then I'll get it there, but most work does not require extreme accuracy.

upload_2016-4-26_8-37-8.png

And the finished part. All of the machining operations are done on the top.

upload_2016-4-26_8-42-35.png

Now to cut the bolt clearance in the bottom. I did this in two setups. The reason I did this in two setups is so I could get a radiused end in both ends of the slot and I didn't have a 5/16 ball end mill that has a 0.75 depth of cut. So rotating 90° solves that issue, and I can make the same shape with a 0.300 DOC. I didn't get any pictures of the setup when cutting the slot in the top, but it was just clamped in the vice with the legs down. Then I rotated it 90° counterclockwise and squared the legs to the vice. Because of the shape of the work, I had to hang it out of the vice quite a ways so vibration will be an issue. To overcome this, I clamped an angle plate to the work to add mass. The angle plate is not bolted to the table, it just adds mass to the system.

upload_2016-4-26_8-52-41.png

And nearly finished

upload_2016-4-26_9-0-18.png

The next operation is to cut the clearance slot for the hinge. For this operation, a HF angle gauge is used, this thing is actually pretty accurate, and the operation does not require extreme accuracy, it's just clearance. First check the angle gauge to see if there is an offset needed, but it's reading right on 0 :)

upload_2016-4-26_9-5-40.png

The work will be done on the right hand side and the work needs to be rotated 28° off of vertical so using the flat surface on the other side the angle can be set. It's the only surface that is parallel with the feet. I figured out how to reset the camera so the pictures are normal again.

upload_2016-4-26_9-11-41.png


So how do you locate the work when there are no flat surfaces to work from? Well there is a nice reamed 0.375 hole with a known location, so stuff an end mill with a 0.374 shank in there and locate off of that.

upload_2016-4-26_9-18-31.png

I am not happy with this setup and the slot shape that will be generated. I need to re-think this before I make chips. o_O That and I need to go get a couple more 1/4 inch router bits.;)

Stay tuned......More later! :)
 
Last edited:

FOMOGO

Active User
H-M Platinum Supporter ($50)
Joined
Sep 2, 2013
Messages
2,005
Thanks for posting the blow by blow account of your steady rest build and all the other useful tips & tricks that go into the process. Mike
 

JimDawson

Global Moderator
Staff member
H-M Platinum Supporter ($50)
Joined
Feb 8, 2014
Messages
7,837
OK, thinking is done and the options have been explored. I could spend a day and a half making up fixturing, writing G-code for the 4th axis, and setting up to make the Ideal Shape, or I can just cut the *&^^ slot an inch deep and do it the Easy Way. I would have had to build a 4 inch riser for the 4th axis, then build all the fixturing, would have been a project worthy of it's own thread. Not gonna happen! o_O Especially when the straight slot will work and I can get it done in about 15 minutes, setup, G-code and all.:oops:
All of this because I did not think through the design before making chips. :burned up::cussing: A little more thought and planning goes a long ways.

So here's what I'm going to do.

upload_2016-4-26_12-43-1.png

OK, off to buy some router bits and run a few errands.

More later........:)
 

Steve Shannon

Rocketgeek
H-M Supporter - Gold Member ($25)
Joined
Nov 27, 2015
Messages
600
I hate to be the first to tell you, but sound travels 330 m/s or about 1075 ft/s at sea level. I always figure lightning is a little over a mile away if it takes five seconds.


Steve Shannon
 
Last edited:

JimDawson

Global Moderator
Staff member
H-M Platinum Supporter ($50)
Joined
Feb 8, 2014
Messages
7,837
Well I can see the light at the end of the tunnel. This was supposed to be about a two day project but so far I'm into it about 10 days and still not quite done. But I may finish it later this evening, it's really time to get on to a couple of other projects.

First set up and cut the slot for the hinge. The big chunk of steel clamped on is just to add mass to to keep any chatter to a minimum because the work area is sticking so far out of the vice. I could have removed the vice and done this with an angle plate but I wanted the vice on for the next operation.

upload_2016-4-27_17-44-47.png

And check the fit before tearing down the setup. The fit is good!

upload_2016-4-27_17-46-55.png

And in the open position

upload_2016-4-27_17-47-28.png


Now to drill and tap the base mounting holes. The dimensions have changed so many times on both the base and the bottom that I no longer know where the screw holes are relative to an edge. So the easiest way to locate the holes is to put the base on the bottom, line everything up, and transfer punch one hole. I know where the holes are relative to each other, just not to an edge. The holes in the base were drilled 1/64 oversize for bolt clearance so it has a little wiggle room.

upload_2016-4-27_17-55-22.png


Then using the pointy end of the edge finder and a thumbnail it's easy to locate the transfer punch divot. If you can't catch a thumbnail on the edge finder in both the X and Y axis (both sides), then you are pretty close to center. The set your DRO to the location of that point, or if you don't have a DRO, that point becomes your zero.

upload_2016-4-27_18-1-15.png


OK, drilled & tapped, and bolted into place. Where possible I drill & tap blind holes at least 1 inch deep, I hate bottoming out bolts. Also, I normally put the spindle in neutral, chuck up the tap, and run it in by hand a few threads. Then loosen the chuck and finish by hand tapping. I normally don't powertap over 1/2 inch deep.

upload_2016-4-27_18-4-42.png

And there it is. Only one assembly left to build. The clamp bolt system. Won't take too long to build and may get done tonight.

upload_2016-4-27_18-9-54.png

Stay tuned.......
 
Last edited:

JimDawson

Global Moderator
Staff member
H-M Platinum Supporter ($50)
Joined
Feb 8, 2014
Messages
7,837
IT'S DONE! :beer bottles:

I went ahead and finished it up tonight.
All I needed to do was make a knob and a swing bolt. Not really much to it but I'll post a couple of pictures showing a couple of tricks.

I made the swing nut out of 2 inch aluminum, turned the shank down to 3/4. I wanted a radius where the thumbwheel meets the shaft. I left enough material to cut the radius out. I've never tried this before, I used a 3/8 ball end mill to cut the radius. Just set the tool on center, with one side of the ball cutting edge at the ''correct'' angle. Went in and took light cuts working back and forth so it didn't try to take the whole radius in one bite to minimize chatter. It worked great! :encourage:

upload_2016-4-27_23-4-5.png

And the finished radius

upload_2016-4-27_23-4-49.png

One trick I use to square the tool holder to the lathe when needed is to just run the holder up against the chuck, move the carriage as needed. and tighten the clamp nut when you get it square.

upload_2016-4-27_23-8-35.png

The only parting tool I own :grin: It has never jammed. Note: DON'T RUN THE SPINDLE when using this type of ''parting tool''

upload_2016-4-27_23-11-17.png

I already drilled & tapped the swing nut, but I wanted to chamfer the other side. So I flipped it over and used the tap drill to align the hole with the spindle so I could chamfer on center.

upload_2016-4-27_23-14-58.png


And here it is, ready to use.

upload_2016-4-27_23-16-24.png

and as I mentioned in my first post in this thread, I built this to hold a 20 inch chunk of 3 1/2 inch UHMW so I can drill a 1 inch hole through it. That project is going to be a little tricky so I'll post when I get to it in the next day or so.

Here it is!

upload_2016-4-27_23-19-24.png

Thanks for looking and I hope someone can find something useful to take from this.:)
.
.
 
Last edited:
[5] [7]
Top