Press Feeder

JimDawson

Global Moderator
Staff member
H-M Lifetime Diamond Member
Joined
Feb 8, 2014
Messages
9,711
Lately my project posts have been few and far between, not because I haven't been doing anything, but rather what I have been doing is protected by NDAs and I'm not allowed to show my work to the general public. I've actually been doing some pretty cool stuff, some of which has very interesting setups, work holding and machining challenges that tax my abilities.

I finally have a project that I can show.

Some of you may remember the servo driven punch press I built for a customer about 18 months ago. https://www.hobby-machinist.com/threads/servo-punch-press.72601/

1582779482822.png


It works OK, but there has been one nagging problem since day one. When the material spool is full, they can't run it at high feed rates because mass of the spool is more than the feed rolls can accurately accelerate. This means that someone has to stand there and spool off the material to keep some slack in the material so the feeder is free to accurately feed the material. I should note that we are trying to hold +/- 0.001 inch or better on feed position and thus the punched hole spacing. That sounds like a crazy tight tolerance, but concider that's 0.1 inch over 100 inches which is bordering on unacceptable. The good news is that the hole to hole actual position is + or - a bit so the average is pretty good.

Since this press is designed to allow variation of the feed length at a push of a button to make different product styles, the longer the distance between the punches means the more mass that needs to be accelerated between the punches, and the press is not able to position accurately at longer feed lengths without operator intervention. So to overcome this problem the customer has commissioned a pre-feeder, similar to a common punch press material spooler.

The goal is to try to keep a constant amount of loop in the material to minimize any feed error at any possible feed rate. And do it all automatically, while being able to feed material from spools staged on a seperate rack system.

Here is the overall concept. This is shown in the rest position, material flow is left to right. The feed arm senses the loop height, and as the the loop height changes, the feed motor speeds up or slows down as needed to try to maintain a constant loop length. The sensor arm is connected to a pot that controls the VFD.
1582783333099.png

I'll post pictures of the pallet of raw materials and parts in the morning. All of the bits & pieces arrived yesterday, and I went shopping today to buy the steel, aluminum, and plastic needed to hang all of the parts on. Then you'll get to see it all take shape over the next couple of weeks.

Not a terribly complex project, but should be fun.

Stay tuned............
 
Last edited:

JimDawson

Global Moderator
Staff member
H-M Lifetime Diamond Member
Joined
Feb 8, 2014
Messages
9,711
I cut all of the material to roughly part sized chunks a couple days ago, and spent yesterday doing all of the CAM work to develop the tool paths.

The first step in the machining process is to make a fixture plate to hold the parts while machining. So a 6x8x5/8 chunk of aluminum will nicely fit in the vice and all of the parts except the main mount plate will fit in that envelope. All of the parts were designed to have hold down holes in them that have no function in the final assembly, only to facilitate machining.

Nothing worse than trying to figure out how to hang onto a part when you start making chips. I ''machine'' all of the parts in my head during the design phase, taking into account work holding and tools required. All of the raw pieces are cut at least 1/4'' oversize to insure plenty of material to cut all the way around.

So first I turn the fixture plate into Swiss cheese, drill and tap all of the needed holes for all of the parts. The the hole dimensions are just to remind me what a particular hole is supposed to be, it would suck to tap a hole 1/4-20 when it was supposed to be 10-24. The hole dimensions are shown as the bolt size rather than the tap drill size.
1582997356780.png

All of the parts have 0,0 located at the top right corner and are offset 1/8 inch from that point.

Here are the gussets overlayed on the fixture plate. It was a little bit of a challenge to place all of the parts and locate the holes so they didn't interfere with each other. These parts are held down with the four 0.250 bolts on the red lines. The fixture plate holds 7 different parts.
1582998102411.png

I may go through and pre-drill all of the pieces, then do the fixture plate last. I think that will be more efficient and I won't have to mess around clamping the pieces down to the fixture plate for drilling. That way, all I have to do is screw down the part and start cutting. The starting location of the workpiece is not critical, anywhere +/- 0.01 or so is fine and I'm pretty sure I can get there. When finished, the final dimensions will be relative to the fixture plate 0,0 point, if the hold down holes are off slightly from the design it won't make any difference because for the most part they have no function other than to hold the work while machining.

.
 
Last edited:

Winegrower

H-M Supporter - Gold Member
H-M Supporter Gold Member
Joined
Jul 29, 2014
Messages
817
This is a good approach. It reminds me of the way a tape tension arm maintains the right pull while a digital tape recorder is going from forward to fast forward to rewind, etc. You drive one reel as master and use tape tension as motor control input for the slave reel.

Oh man, I am speaking of antiquities here.
 

JimDawson

Global Moderator
Staff member
H-M Lifetime Diamond Member
Joined
Feb 8, 2014
Messages
9,711
Here is all of the material roughly cut to size.
1583034751457.png

I got all of the part blanks drilled for mounting and the fixture plate drilled & tapped. That's enough for one day.
1583034783301.png

Machine 0,0 is set at the top right of the fixture plate, this will not change until all of these parts are complete. The bolt holes in the blanks will set the blank to the top right.

I'll take a facing cut on the fixture plate in the morning just to make sure it's flat. Then it's time to make chips.
1583034821562.png
 
Last edited:

mmcmdl

H-M Supporter - Diamond Member
Staff member
H-M Lifetime Diamond Member
Joined
Jan 31, 2016
Messages
3,502
Looks cool . I used to love making this kind of stuff . I take it the middle roller is the " dance roller " ? Most of our lines are equipped with either dance roller sets or accummulator rollers that keep the tension at a desired set point . Occasionally , the operators would thread the material wrong and we had a mess on our hands ! :big grin:
 

JimDawson

Global Moderator
Staff member
H-M Lifetime Diamond Member
Joined
Feb 8, 2014
Messages
9,711
Looks cool . I used to love making this kind of stuff . I take it the middle roller is the " dance roller " ? Most of our lines are equipped with either dance roller sets or accummulator rollers that keep the tension at a desired set point . Occasionally , the operators would thread the material wrong and we had a mess on our hands ! :big grin:
I have never heard the term ''dance roller'' before, but yes, that is what it does. That arm is connected to the pot that controls the VFD.
 

mmcmdl

H-M Supporter - Diamond Member
Staff member
H-M Lifetime Diamond Member
Joined
Jan 31, 2016
Messages
3,502
I think we all call them dance rollers because they seem to " dance " while running . We made sets for shrink sleeve machines that would accumulate 5 minutes worth of run time when the rolls ran out . The operators had 5 minutes to splice the new rolls to the expiring rolls , thus the line never stopped . :encourage:
 

JimDawson

Global Moderator
Staff member
H-M Lifetime Diamond Member
Joined
Feb 8, 2014
Messages
9,711
I think we all call them dance rollers because they seem to " dance " while running . We made sets for shrink sleeve machines that would accumulate 5 minutes worth of run time when the rolls ran out . The operators had 5 minutes to splice the new rolls to the expiring rolls , thus the line never stopped . :encourage:
We used to do that with the rolled roofing line I used to run, about 50 years ago. Had big accumulator systems on the infeed and outfeed of the machine, depending on the product we were running, we would have 3 or 4 minutes to make the splice. Used a flat iron and some kind of heat sensitive cloth tape.
 

mmcmdl

H-M Supporter - Diamond Member
Staff member
H-M Lifetime Diamond Member
Joined
Jan 31, 2016
Messages
3,502
Exactly ! I wish I had the knowledge you have of the electrical ends of these machines .............................................





I would be " dangerous " . :grin:
 

JimDawson

Global Moderator
Staff member
H-M Lifetime Diamond Member
Joined
Feb 8, 2014
Messages
9,711
always a pleasure to follow your projects Jim, I never fail to learn something new!
Thank you Matt.

Well another day and a few more chips.

Here is the bracket blank screwed to the fixture plate.
1583116848388.png

And in process. First remove the material between the parts because not doing so will result in a small bit of material that is floating around that could jam somewhere and potentially break a rather expensive end mill. More on breaking expensive endmills later. :rolleyes:

I'm always amazed at the fast shutter speed of my cheap little camera. That spindle is turning 2200 RPM in this picture, no motion blur at all.
1583117260901.png

And profiling the outside of the parts
1583117361052.png

And finished, about 18 minutes run time. The endmill path around the part is just visible, you can't catch a fingernail on it. Almost not there.
1583117465427.png

Then on to the next piece. It cut the two 3/8 slots perfectly then rapid over to do the outside profile and SNAP o_O A brand new 3/8, 3 flute, solid carbide, aluminum cutting Onsrud endmill (about $45). It won't cut 1/8 deep at 100 IPM and that RPM. I was looking at the G code on the screen just before this happened and saw it coming and was already moving to the E-stop , but I wasn't fast enough. :faint:
1583118173774.png

The problem was caused by a programmer (me) malfunction. The clearance height was supposed to be set at 1.5 inches, NOT 0.5 inches. 1.5 inch clearance height will be needed for a later part, would not need that much for this particular part but it saves confusion when everything is the same. The tool needs to clear the top of the material, plus the height of the hold down screw heads. In this case, 0.5 inches clearance height puts the tool 1/8 inch INTO the 5/8 thick material.:eek: In my defense, I have my default clearance height set at 0.5 inches because I normally set Z zero to the top of the work, but in this case where I have a common fixture, I have Z zero set to the top of the fixture plate or the bottom of the workpiece which works out fine when working with material of different thicknesses, as long as the clearance height is set correctly for the operation.

Things can go south in a hurry on a CNC machine. I really hate it when the machine does exactly what it's told to do rather than what I want it to do. :grin:

I have gone through all of the CAM operations and made sure the clearance heights are set correctly. Anyway, grab another $45 end mill out of the drawer, stuff it in the holder, re-zero, and finish the part. I can save the part, a little surface blemish is not a problem, and that surface will be hidden when installed.
1583119648130.png

More tomorrow...... Stay tuned
 

mattthemuppet2

H-M Supporter - Gold Member
H-M Supporter Gold Member
Joined
Sep 28, 2013
Messages
2,263

JimDawson

Global Moderator
Staff member
H-M Lifetime Diamond Member
Joined
Feb 8, 2014
Messages
9,711
bugger! The best lessons are the most expensive, right?

Would something like the following work as replacements? I have quite a few YG-1 endmills and they work really well. no different to Niagara or other major brands in my hands.

Might be worth a look, for roughly the same end mill there is about a $4 price difference.
 

JimDawson

Global Moderator
Staff member
H-M Lifetime Diamond Member
Joined
Feb 8, 2014
Messages
9,711
I didn't get a lot done yesterday, just one part machined. First I had to get my truck into the transmission shop for a rebuild, second gear was pretty much gone. A typical problem for Dodge Diesels with around 180K miles. I don't have enough energy to do it myself, and we have a local shop that does it right.

Then I got home and started setting up the next piece to machine, did an air cut and the machine randomly hung on a transition. That's not good, go into the program to figure out what was happening. Found the problem, I made a program change a couple weeks ago to smooth out the operation, well I created a new problem when I did that. Typical programming issues. About an 1 1/2 hours later I figured out how to fix the problem and ran a few more air cuts to make sure everything was going to behave.

Then spend the next hour or so setting up the lathe for the next run of parts.

Finally I got around to making chips for this project.

1583268308957.png

By this time it's about 6:00 PM and I'm tired. Not to mention I ran out of propane for my heaters. So done for the day. And today I have to wait for my son to get here with his truck so we can go get propane, so haven't gotten much done today either.

And now I have some stupid scammer pop ups on my computer telling me that my computer has a virus, I wish I had time to screw with these guys. I have some ''special'' software that they would get when they connected to my computer. It will turn their computer into a brick, don't mess around with an old programmer. Time to clean my computer. I don't think I'm going to get a lot done on this project today.
 

JimDawson

Global Moderator
Staff member
H-M Lifetime Diamond Member
Joined
Feb 8, 2014
Messages
9,711
More fun and games. Got a couple more parts roughed out today.

This is where the pucker factor goes up a bit o_O , 3/16 slot, 5/8 deep with a 1/8 inch end mill.
1583428121160.png

I was distracted when I was setting this up so forgot to turn down the feed speed. I had it set for about 6.5 IPM and it should have been 3.5 IPM for these conditions. But it still made it through 1 slot and about 95% of the second one. So I'm happy. Used a racetrack spiral down tool path.

1583428337489.png

And the part on the left semi-finished as is the bore on the right part.... Why semi-finished? Because the center pocket is a bearing bore and I'm having a problem interpolating a round hole, it's 0.002 out of round. I expected that so left the bore 0.010 undersize. I'll bore it in a later operation. I need to work on my servo tuning to correct this. I can't find any backlash in the machine.

1583428891547.png

And done. This is all I got done on this project today due to other interruptions, about 40 minutes of actual machining time.
1583429016506.png

At the same time I was trying to run this part, I was also making parts on the CNC lathe and was having material feeding problems. The ''precision'' ''1.500'' inch round bar stock we bought isn't very precision. It actually measures 1.507 and won't feed properly through a 1.500 collet. So tear down that setup and change over to another product that will feed through a collet. I'll put the chuck on the lathe to run the 1.5 inch parts, there is always a workaround. The bar stock we bought is American made by Kaiser Aluminum, not sure if it is in spec or not. Doesn't matter, we'll use it anyway, but will let our vendor know.

On another note, I got my truck back from the transmission shop, Trans-Medic in Gresham for you local guys. It seems to work fine now, actually shifts. :encourage: They do good work and I recommend them.

Don't know how much work I going to get done on this project today, I need to go to a customer and make some control modifications to a large CNC router. Too many projects at the same time.

More later....... Stay tuned.
 

mattthemuppet2

H-M Supporter - Gold Member
H-M Supporter Gold Member
Joined
Sep 28, 2013
Messages
2,263
you sure do keep yourself busy Jim :) I'm surprised there wasn't much of a difference with the YG-1 endmills, though I'm guessing you use a long LOC than the one I posted.

When you say you got 95% through the 2nd slot, what happened with the last 5%?!

I won't bore you with what I did today, it was miserable and stressful!
 

JimDawson

Global Moderator
Staff member
H-M Lifetime Diamond Member
Joined
Feb 8, 2014
Messages
9,711
you sure do keep yourself busy Jim :) I'm surprised there wasn't much of a difference with the YG-1 endmills, though I'm guessing you use a long LOC than the one I posted.

When you say you got 95% through the 2nd slot, what happened with the last 5%?!

I won't bore you with what I did today, it was miserable and stressful!
1 1/4 inch LOC, same as the YG-1.

The end mill broke before it finished the last 5%. Not a problem, it's just screw slot. I can finish it out with a die grinder in a few seconds.

Oh, and the control mod on the router was just moving a wire to another terminal. About 10 seconds. And about 10 minutes to figure out which wire to move and where to. The travel time was considerably more than the on-site time, they'll be billed for both.;)
 

JimDawson

Global Moderator
Staff member
H-M Lifetime Diamond Member
Joined
Feb 8, 2014
Messages
9,711
I got a little more work done. Trying to setup and run two machines is a little taxing, and the lathe parts run is the priority right now. The press feeder is more of a fill in at the moment..... Until it becomes a panic. :)

This is the slide plate that holds the pressure roller. You'll see how all of this goes together later. It was a little exciting going 3/4'' deep in steel with a 1/8'' end mill to do the finish profile to clean up the corners in the center slot. The bulk of the material was removed with a 3/8, 4 flute carbide endmill.

1583692890063.png

This is the bearing housing and adapter plate for the motor adapter.
1583693079133.png

And one side finished along with the adapter (purchased from McMaster).
1583693134576.png

And it fits :)
1583693259970.png

Now I have to flip the bearing housing over and machine the bearing pocket. So this requires a clearance pocket in the fixture plate. This pocket also locates the part exactly on the center so I don't have to re-zero.

1583693498087.png

Or at least it should work that way. I'm having a bit of a problem with my machine: When cutting a circle, my Y axis dimension is always 0.002 smaller than the X axis dimension and this problem is getting worse, it used to be 0.001'' difference. When cutting a rectangle, the X and Y dimensions are always correct to +/- 0.0001''. I can't find any backlash in the system, and the math that calculates the circle seems to be correct in the program. I suspect a servo tuning problem, but not sure. I need to take a deep dive into this to figure out. For the moment, I can bore the critical dimensions to the correct size in a second operation, I left them undersize to accommodate the known error.
 

JimDawson

Global Moderator
Staff member
H-M Lifetime Diamond Member
Joined
Feb 8, 2014
Messages
9,711
Haven't updated in a few days.

I finished up the secondary operations on most of the parts so they are complete. Just need to bore the bearing bores to final size, this will be done on the lathe. I'll be starting on the turned parts in a day or so, just need to finish up the mill work.

So here are the completed parts. The vise was on the machine when starting this project so I did all of the work that could be held in the vise first.
1584159989784.png

First today I need a 5/16-18 hole tapped at about where the point of my scribe is. A little tricky to drill & tap a hole in that location so is going to require some special tools.
1584160241610.png

So set up on the angle plate and grab a long tap size drill bit. This is about the lower limit of my table, and the 5'' of quill travel is about 1/2'' into the work.
1584160602290.png

So get the drill bit started in the hole, then raise the knee to finish. I went down until the chuck just about touched the work., I don't like short holes when tapping, I want lots of room where possible.

1584160821500.png

After drilling the top hole to size, clearance for a 3/8'' screw, I thought I was going to use this tap. But it turned out that the tap would not even get a good start in the hole without getting tight, and I wasn't about to force it. Don't need a broken tap in a blind hole and in the bottom of a slot. So find plan ''B''
1584161082103.png


The tap looked fine and felt sharp, not sure what was going on with it. So the next step is to figure out how to extend a standard spiral point tap so I can turn it. A 5/16 tap has about a 1/4'' square drive end, so a perfect fit for a 1/4 drive socket extension. My 1/4'' drive socket extensions would not fit down a 0.400'' hole and I couldn't find a short one the I could get in there, and I wasn't about to modify one of my good extensions. Nor could I find a 12 point 1/4'' socket. So into my misc. tool drawer to find something that would work.

This is a bunch of mostly cheap wrenches, as well as duplicates that I have collected over the years. I couldn't find a 1/4'' drive extension, but I did find a 1/4 drive, 1/4'' 8 point socket. OK, now I'm in business, got the hole tapped. All this hole does is hold a 3/8 headless shoulder screw for use as a guide pin.

1584161928709.png

Then onto the next setup, the main mounting plate. A big ugly 1'' thick chunk of steel roughly 6x19''
1584162591752.png

First order of business is to cut it down to 6 1/4'' wide from the original 8 inch wide. My old $25 bandsaw got a bit of a workout today. It really didn't take that long to do, about 15 minutes, even with a tired blade.

1584162908022.png

Then over to the mill to make swiss cheese out of it. All drilled, tapped, and counterbored as needed.

1584163060499.png

This was not without some frustration. Broke a 5/16-18 tap buried about 3/4'' into a hole.
First I tried a punch to try to turn the tap, it turned about 1/4 turn and just stopped. I figured it would do that.
So next I tried a worn out solid carbide spotting drill, it kind of wore a divot in the top so I had a bit of a guide for the next try.
A carbide masonry bit just wanted to walk to the side, so that didn't work.
So I grabbed a 1/4'', 3 flute, solid carbide endmill (bottom tool in the picture), and managed to chew through the tap. Even saved the threads, and didn't hurt the endmill much either.
1584163217212.png


Tomorrow I'll do the milling on the plate, and that will finish it up. Then only one more piece to do on the mill, and then do some turning work and I can put it all together.
 
Last edited:

mmcmdl

H-M Supporter - Diamond Member
Staff member
H-M Lifetime Diamond Member
Joined
Jan 31, 2016
Messages
3,502
Those clamps always show up in the worst places Jim ! :grin: Pretty cool hitting them at 400 ipm in a rapid move and knocking an inch or 3 off your end mill . :bawling:
 

JimDawson

Global Moderator
Staff member
H-M Lifetime Diamond Member
Joined
Feb 8, 2014
Messages
9,711
OK, moving right along.....

I finally found time to fire off the mill again and rough out the outside profile and bearing pocket in on the main mounting plate. One thing of note is that I took a cut with a partly worn out roughing endmill on the one edge that was so far untouched and had the original finish. I did this to preserve my new rougher that I intend to use for the roughing work, it would have been damaged by the mill scale on the first pass.

The mill scale on hot rolled steel is like carbide, really hard on tools. So I took about a 0.050 width of cut by the full 1 inch depth and cut in the conventional direction rather than a normal (for CNC work) climb cut. This allowed the tool to get under the scale and approach it from the back side so the tool was not trying to dig into the scale as the tooth approached the work. A couple of other ways of removing the mill scale is to simply saw off the edges or by grinding down to bare metal. In this case, I'm leaving the mill scale on the front face because I want the hard surface for an anti-wear bearing surface, and on the back side it doesn't matter anyway.

First pass with the rougher, 1'' DOC, 0.050'' WOC, 1/2'', 4 flute, cobalt roughing endmill, 94 FPM (about 740 RPM), and about 0.0019 feed / tooth, 5 IPM.

1584332520142.png

And cutting the indents. The indents are really only for appearance in the finish part, no useful function. Same cutting parameters as above.
1584332696715.png

Here are the tool paths, each yellow line represents one pass and is the center of the tool, the blue lines are rapid moves. 0,0 is the top right corner, at the edge of the raw stock, and this was a mistake on my part as you'll see below.
1584333103888.png

And the outside rough profile finished, I left 0.020'' on each side for finishing. And have moved over to rough out the bearing pocket. About 90 minutes of cutting time so far.
1584333554907.png

Same cutting parameters as above except for the DOC was set to 0.300 to allow for chip removal with the mist coolant system. I didn't want chips packing in as they would have done had I gone the full 1'' DOC.

Now comes the fun....... POWER FAIL :eek: for about 1/2 hour. And the only time I lose my zero is on a complete power down.

Yup, as I said above I put the 0,0 in the wrong place, that point is gone, it's in that pile of chips. :bang head: Worse yet is I'm not even exactly sure where any feature is at relative to the existing edges because they are not finished and are of a bit indeterminate size because the end mill was a bit smaller than 1/2 inch and the material was cut ~1/8'' oversize all around and I zeroed on the raw edges.

What could I have done differently? I could have put a small divot in the part at a known location with a center drill when I was drilling all of the holes and used the pointy end of the edge finder to locate that divot. I could have relocated in a couple of minutes.

This is the position that a power fail left the tool in............. So how to zero on a point in space?
1584334182413.png

So back to the drawing and locate the bearing pocket from where the computer thinks it is.

1584336612610.png

Which is located at -9.657, -3.125, so now all I need to do is locate the center of the pocket and plug those numbers into the program. So bring out the Blake center indicator, and warm it up in front of the heater. It doesn't like to work when its cold. Found the center, plugged in the numbers and I'm back running.
1584337154423.png

By this time it's about 7:00 PM, so I'm done for the day. Tomorrow I'll finish cut the outside profile and finish bore the bearing pocket, then this part will be complete.
 
Last edited:

JimDawson

Global Moderator
Staff member
H-M Lifetime Diamond Member
Joined
Feb 8, 2014
Messages
9,711
I got one chunk of iron off of the table and time to load another. Need to make a few holes. Didn't get a whole lot done today on this project, had to do some programming work, and then to set up the lathe for the next run.

I put all of the holes on one side of the drawing, but they will actually be on 3 sides, but all relative to the same 0,0 point. Just makes easier to do one CAM setup.

The most fun one will be the two inch hole. It has to align on both sides of the 4 x 4 x 1/4 wall tube, the rest of the holes are just drilled & tapped in one wall. I'll do the 2 inch hole from one side, probably with a long endmill. Drill first, then run a pocket routine. I could use a hole saw then bore, but I don't have a good way to hold the holesaw arbor. Keyless chucks can be destroyed by over torque and a hole saw is way over the chuck's capacity. I have one on the bench that was damaged that way, not sure if I can fix it. I don't have a keyed chuck for the mill, guess I should buy one.
1584417771347.png

About 39 inches long, pretty much takes up the whole table but all of the work is within about a foot of the end, just need room to support it.

1584418032195.png

Since there is nothing critical in the hole locations except that they need to be relative to each other, using a square to align to the table is close enough, this normally gets me within a couple of thou. No dialing in required.

Just move the scale to the work and lock the screw. And snug the clamp down.

In the upper left of the picture, you can see the magnetic scale coming loose from the table. This has been on there since 2014. I spilled some MEK in that area about a year ago, other than that, the tape seems to be impervious to any coolant and way oil. I have some new strip I'll install when this project is complete. Only takes about 15 minutes to install.
1584418759772.png

Then move the other end to the scale and snug that clamp. Check the first end again and tighten the clamps.
1584418886609.png
 

JimDawson

Global Moderator
Staff member
H-M Lifetime Diamond Member
Joined
Feb 8, 2014
Messages
9,711
Got the holes done on one face of the tube before I had to set up the lathe again.

The 1/2 and 10-24 tapped holes went fine, then was time for the 2 inch holes through both faces. That took a bit of thought. I decided to go with the long end mill method.

First I drilled through with a 3/4'' drill just to get a starter hole. Then machined the top hole with a 3/8 solid carbide, 4 flute end mill.

I since I haven't made the mating part yet, I decided to make the top hole 2.062 rather than 2 inch. This will give the long endmill some clearance on the shank when doing the bottom hole, and allow easier insertion of the mating part.
1584505495404.png

So now it's time to pocket the bottom, so out comes the 3/4 inch, 4 inch cutting length, 4 flute. This pretty much used up all of the quill travel I have.

1584505807662.png

I rigged the coolant up inside of the tube so I could get it where it would actually do some good.
1584505914215.png

And the inside view
1584505958864.png

And away we go, running a pocketing routine. Spiral down in the center, then 0.050'' DOC and 0.050'' step over. Not much quill travel left.
1584506987503.png

An an inside shot, that's a lot of endmill hanging out there. :cautious: But everything went smooth with minimal chatter.
1584506302253.png

And a screen shot of the cutting parameters.
1584506375310.png

I'll get the other 6 holes drilled & tapped tomorrow then that will end the mill work, other than possibly some minor adjustments on this project.

Then it's over to the lathe to make a few pieces.

Stay tuned..........
 
Last edited:

JimDawson

Global Moderator
Staff member
H-M Lifetime Diamond Member
Joined
Feb 8, 2014
Messages
9,711
Finished up that big ugly 4x4 tube this morning and that completed most of the mill work on this project.

So over to the lathe to make round things. The other day I did a quick install of a new magnifier lamp for the lathe. Well, it was a little too quick, kinda had a small problem :eek:
1584588319097.png

I didn't check for clearance between the lamp mount and the tailstock. OOPS. :bang head:
1584588448160.png

So rotate the bracket 90 degrees and fixed for the moment. I think I need to do something else here, not sure if I like this mount. We'll see by the end of this job.
1584588537163.png

The view through the magnifying lamp, actually works pretty good. This is about what it looks like to me also. Much easier on the old eyes.
1584588847132.png

First I turned down a chunk of 1 3/16 steel to 1 inch, leaving 1 inch of it at 1 3/16. Normally would not even be noteworthy but it is a part of the project and has a dual use as a fixture.

The finished shaft that will double as a stub arbor for the next part. About 8 1/2 inches long
1584588957235.png

So the next part is the bushing that the shaft rides in, 4 inch UHMW. I drilled and bored through for a 0.002 clearance fit on the 1 inch shaft. Now I have to turn the OD to 2 inches to fit the hole that it goes in. And the OD needs to be more or less concentric with the bore which means I need to mount it on an arbor to turn the OD. This is where the above shaft come in.

First drill & tap 1/4-20 for a drive pin (1/4-20 screw).
1584589407671.png

Then put the shaft in chuck and drill & tap the end for 1/2-13. Then slide on the UHMW with the drive screw in it.
1584589548470.png

The drive pin engages the chuck jaw to turn the part.
1584589615896.png

I chucked the shaft just a bit short of the length of the UHMW so the end screw would hold it to the chuck jaws.
1584589740881.png

Then center drill the screw a bit to get a decent center
1584589823779.png

And ready to make piles of nasty UHMW stringy things.
1584589895114.png

That's all there is for today...... stay tuned for more.
 

JimDawson

Global Moderator
Staff member
H-M Lifetime Diamond Member
Joined
Feb 8, 2014
Messages
9,711
Finished up the UHMW bushing and bored the timing sprocket that will live on this shaft.
1584675024004.png

Then faced and bored the drive roller.
1584675093639.png

And because of many other tasks, this is all I got done today on this project. I'll finish the drive roller tomorrow, and get the main drive shaft completed. Then back onto the mill for a few odds & ends that need to be finished. Maybe I'll get the stand welded together and painted over the weekend. Then when I get the aluminum parts back from anodizing (Monday maybe?) I can start assembling.
 
It can take up to an hour for ads to appear on the page. See our code implementation guide for more details. If you already have Auto ad code on your pages there's no need to replace it with this code
Top
AdBlock Detected

We get it, advertisements are annoying!

Sure, ad-blocking software does a great job at blocking ads, but it also blocks useful features of our website. For the best site experience please disable your AdBlocker.

I've Disabled AdBlock