• This site uses cookies. By continuing to use this site, you are agreeing to our use of cookies. Learn more.
[4]

Building a High Speed Punch Press

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

JimDawson

Global Moderator
Staff member
Director
Joined
Feb 8, 2014
Messages
6,458
Likes
4,436
#1
I normally don't get to post customer projects but I can in this case, nothing proprietary here. I just can't tell you exactly what it's for or show the tooling.

So what do you get when you combine about 150 lbs of steel, a high quality Harbor Freight 1 ton arbor press, a NEMA 42, 4200 oz-in stepper motor, and some electronics?

If I do it right, it will become a variable speed, 600 stroke per minute, 5/16 stroke, 1/4 ton punch press.

First you're gonna say that nobody in their right mind would use a HF press for the base, and I would have to agree. It wasn't my choice, but the customer insisted since he is currently using a HF 1 ton for the job and operating it manually. He wanted to keep the manual capability in case of a mechanical or electrical breakdown so I had to design around that. It will switch over to manual in about 15 seconds, you just have to install the pinion shaft. I suspect the HF press will break long before my hardware.

Here is what it's supposed to look like when it's done.

Press.jpg

The stack of parts. The motor weighs more than the press frame.
IMG_0495.jpg

I'll post pictures of the build as it progresses. The first order of business will be to get the mating surfaces on the press squared up so I can use them.

IMG_0495.jpg Press.jpg
 
Last edited:

Andre

Active User
Active Member
Joined
Apr 28, 2014
Messages
2,104
Likes
582
#2
Seems like a very interesting build, can't wait for more updates.
 

mattthemuppet2

Active Member
Active Member
Joined
Sep 28, 2013
Messages
1,530
Likes
753
#3
awesome, thanks for posting this up! It sounded like a super cool project when I saw it in your shop and it'll be fun to follow it along :)
 

Bill C.

Active User
Active Member
Joined
Mar 11, 2013
Messages
1,387
Likes
152
#4
I normally don't get to post customer projects but I can in this case, nothing proprietary here. I just can't tell you exactly it's for or show the tooling.

So what do you get when you combine about 150 lbs of steel, a high quality Harbor Freight 1 ton arbor press, a NEMA 42, 4200 oz-in stepper motor, and some electronics?

If I do it right, it will become a variable speed, 600 stroke per minute, 5/16 stroke, 1/4 ton punch press.

First you're gonna say that nobody in their right mind would use a HF press for the base, and I would have to agree. It wasn't my choice, but the customer insisted since he is currently using a HF 1 ton for the job and operating it manually. He wanted to keep the manual capability in case of a mechanical or electrical breakdown so I had to design around that. It will switch over to manual in about 15 seconds, you just have to install the pinion shaft. I suspect the HF press will break long before my hardware.

Here is what it's supposed to look like when it's done.

View attachment 94132

The stack of parts. The motor weighs more than the press frame.
View attachment 94131

I'll post pictures of the build as it progresses. The first order of business will be to get the mating surfaces on the press squared up so I can use them.

Hope you can share what the die set looks like. Nice project.
 

Karl_T

Active User
Active Member
Joined
Oct 14, 2014
Messages
887
Likes
328
#6
Jim, interesting project.

With the advent of laser, industry is GIVING away punch presses. Why didn't the customer want to just get one of these?
 

JimDawson

Global Moderator
Staff member
Director
Joined
Feb 8, 2014
Messages
6,458
Likes
4,436
#8
Jim, interesting project.

With the advent of laser, industry is GIVING away punch presses. Why didn't the customer want to just get one of these?

I tried to talk him into a little Benchmaster OBI or something like that, but this is what he insisted on.:nuts:
 

JimDawson

Global Moderator
Staff member
Director
Joined
Feb 8, 2014
Messages
6,458
Likes
4,436
#9
OK, I have one side of the press prepped for mounting my hardware.

Here is how I decided to hang onto it while I'm making chips.

I put the ram in the vice and indicated it in. Then I slid the press over the ram and tightened the ''gib'' screws. This puts everything else relative to the ram ways. This should give a repeatable locating method. Sometimes finding a starting point on a casting is a challenge. I supported the bottom of the press by clamping it to an angle plate. Then I put a jack screw under the web that I will be machine on. This made for a very solid setup.
IMG_0496.jpg

IMG_0502.jpg

A quick cut on the top of the pinion bearing just to square it up, I took off just enough to clean it up
IMG_0498.jpg

All of the dimensions are taken from the center of the pinion bore, so the next step is to center on the bore with the co-axial indicator.
IMG_0499.jpg

Prior to this I had no easy way of figuring out the radius of the flange on the pinion bearing or accurately locating it but once I knew where the bore center is, then I could find the edge of the flange with an edge finder. Once I had this information, I updated the drawing and prepared the g-code file to actually do some work.
IMG_0500.jpg

The first cut is to run a pocket routine to get a flat surface to mount the side plates. The surface was surprisingly flat, only out about 0.017 out. The outside of the flange was actually thicker than the inner part. I expected it to taper the other way.
IMG_0503.jpg

This takes confidence in the G-code and the machine accuracy, the endmill clears the vice by 0.015. I also did an air cut to confirm the clearance.
IMG_0505.jpg


The next step was a bit hairy, a 0.250 solid carbide end mill hanging out of the collet about 2 inches, a spindly little thing. This cleans up the flange radius so I have a locating point for the side plate. Wrapping the side plate around the casting a bit will strengthen the mount and take some load off of the attaching cap screws. The side plated will be stressed vertically in operation. IMG_0506.jpg

Once I completed the work, I milled a small flat on the back of the web for a datum point. I noted the location on the drawing so when I flip the press over I can locate off of the top, and that milled data point. That way if the pinion bore on the other side is not in line, I will still have known points to work from so my flanges are in an identical location on each side and everything lines up properly when I assemble the power head.

IMG_0508.jpg

Stay tuned for more fun!

IMG_0506.jpg IMG_0505.jpg IMG_0503.jpg IMG_0502.jpg IMG_0500.jpg IMG_0499.jpg IMG_0498.jpg IMG_0496.jpg IMG_0508.jpg
 
Last edited:

JimDawson

Global Moderator
Staff member
Director
Joined
Feb 8, 2014
Messages
6,458
Likes
4,436
#10
A little more work on the press project

I flipped the press over and did the machine work on the opposite side, everything was held as in the first side above.

First set Z zero at the highest point that the tool could run into. Then set the clearance plane and Z park 1/4 inch above that. Z always parks before X -Y rapid move. That way when the table rapids to the assigned park position, and it won't smack the tool into something if I screwed up the tool path somewhere.

IMG_0509.jpg

Then find the height of the working surfaces using the tool as a probe. Put these numbers into the CAM program to set the Z positions.

IMG_0510.jpg

IMG_0511.jpg

Flattening out the web

IMG_0513.jpg

Once that was completed I had 3 parts to make out of 3/4 inch C1018 steel

When I design a part, if possible, I will line up any holes with the T-slot spacing in my mill table. In this case it worked out perfectly. I have a drawing of my mill table, and do an overlay to position the parts on the table.

Milltab.bmp.jpg

This is how I set my material.

First I center the spindle on a T-slot I will be using and set the DRO to the dimension on the drawing. It just has to be close because I always move the finished part back from the edge of the material a bit where possible. If it needs to be precision, I will make it precision by locating the T-slot with an edge finder and scribe the line with a height gauge and use my microscope in the spindle for positioning. It is rare that I have to do that. In this case I had over a 1/16 to work with, good as a mile. The old calibrated eyeball is close enough for this setup.

The drill bit is actually centered in the T-slot, the shadows make it look like it touching on the right.

IMG_0514.jpg

Then I set my square to the dimension on the drawing and scribe a line .

IMG_0518.jpg

IMG_0519.jpg

Now I move the material so the scribed line is under the center of the spindle. Again this only has to by close. Then I use the square to set the other end of the material to the same distance from the edge of the table. Then tighten the clamps.

IMG_0520.jpg

Once clamped down, I check the 0 edge for position. Looks good to me.

IMG_0521.jpg

Now I can drill all of the holes and install the hold down bolts. Center drill, pilot drill, drill, tap, and ream as needed. Once the material is bolted down, the clamps are removed.

IMG_0522.jpg

The first part has been roughed out, working on the third part. I am doing it in this order so there will be clearance for the loose pieces when they are cut off. The 1/2 cap screws are bolted through the 3/4 inch MDF backer and into the T-nuts. The two 3/8 cap screws on the left are just threaded into the MDF to keep the part from twisting, I could only put one hold down bolt in that part.

IMG_0529.jpg

All of the parts roughed out. 3/8 cobalt rougher endmill, 0.25 DOC, 2 IPM feed, and 120 FPM (1400 RPM) on the spindle. I probably could have gone through it in one pass with a 0.75 DOC and a higher feed rate, but I wasn't in that big of a hurry. I try to plan my tool paths so the loose piece coming off will not get jammed somewhere. I leave 0.025 for cleanup on a finishing pass, in this case with a 4-flute, 7/16, very high quality end mill from Harbor Freight.:lmao: Out of 3 new ones, I actually found one that was sharp.

IMG_0531.jpg

Finishing pass is done, and the holes have been counter sunk. I do the countersinking on the drill press, the counter sink pretty much just lives there in the chuck, much faster than doing it on the mill unless I need precision.

Here is kind of how everything fits together so far. I need to machine a pocket so the motor mount will clear the edge of the web on the press frame, then it will mate up to the side plates.

IMG_0534.jpg

There will be a motor mount pocket and a bearing pocket machined in where the hold down bolt hole is at right now. That is tomorrow's project.

IMG_0509.jpg IMG_0510.jpg IMG_0511.jpg IMG_0513.jpg Milltab.bmp.jpg IMG_0514.jpg IMG_0518.jpg IMG_0519.jpg IMG_0520.jpg IMG_0521.jpg IMG_0522.jpg IMG_0529.jpg IMG_0531.jpg IMG_0534.jpg
 
Last edited:

Karl_T

Active User
Active Member
Joined
Oct 14, 2014
Messages
887
Likes
328
#11
Always interesting to see how an expert does a job...

Couple questions

Looks like you are machining dry - why?

I've always used AL plate or stand off blocks to mount to a mill for this type application. Any advantage to wood/mdf or just cost? I'd always assumed wood chips, steel chips, and coolant to not work and play well together.

Karl
 

JimDawson

Global Moderator
Staff member
Director
Joined
Feb 8, 2014
Messages
6,458
Likes
4,436
#12
Expert? Not sure about that, but thank you Karl.

In the cast iron of the press frame, yes, I was cutting dry. Most cast pretty much self lubricates due to the free carbon content. Sometimes I use an air blast, but in this case, I just used the shop-vac to suck up the chips.

In the steel, I was not machining dry. There is a mist there, you just can't see it in the photos. My no-fog mister works pretty good, pretty much adjustable between 0 and flood. In this case I was using WD-40 because that is what I had in the tank. I need to build another tank system so I can switch between coolants. I machine a lot more AL than I do steel.

Absolutely cost, MDF is cheap. Like you I use AL plate and/or standoff for production work. But for one-off parts, MDF works great. It's dimensionally stable when well supported. MDF is pretty tough stuff in compression, and drills and taps OK to keep parts from moving laterally, in tension it's not very good, but for light milling using deck screws to hold the part down it works well. It resists coolant pretty well in the short term and I normally use minimal coolant.
 

Reeltor

Active User
Active Member
Joined
Nov 18, 2014
Messages
739
Likes
313
#13
Very interesting discussion about using MDF under the work to be machined. I'm looking forward to hearing more.

Mike
 

JimDawson

Global Moderator
Staff member
Director
Joined
Feb 8, 2014
Messages
6,458
Likes
4,436
#14
A bit more work on the press project today


This is the front support plate. It will have a bore for a ball bearing and some clearance milled for the cam follower carrier. Again this is mounted up on a chunk of MDF and through bolted to the T-slots.


I could cut the parts with the bandsaw, square them up, locate the edges precisely, then drill the hole pattern, or just do all of those operations in one setup. This could be done the same way on a manual machine as a CNC. For the bearing bore and the other machining I will put them in the vice.


IMG_0537.jpg


The next batch of parts is made of 0.500, C1018 steel. There are 5 pieces: 2 side plates, 1 top plate and a pair of cam follower carriers. Again I could have done all of separately, but there are less steps and fewer tool changes when doing them all at once in one setup. There will be a secondary operation on the cam follower carriers to bore the pin hole, but that will be done once they are welded to the ram. I was able to put in ‘’lubrication access holes’’, which just happened to exactly fit the T-slot spacing.:whistle:


I set up the material as I described in a previous post. The one addition that I did here is to put a small mark with a center drill at a known location for a datum point. We had pretty good winds today and I was afraid that we might lose power. This is the down side of using this method to place the material in that I have no idea exactly where the edges are at with out actually measuring. Thus the witness mark in case I lose the 0. I could locate this mark with either the pointy end of an edge finder or a spindle microscope.


IMG_0551.jpg


IMG_0550.jpg




First center drill and pilot drill, and final drill the hold down cap screw locations, then install the hold down bolts.


IMG_0552.jpg


Then center drill and pilot drill, and final drill the rest of the holes. The 3/8 and ¼ inch cap screws are threaded into the MDF. Because there is only one hold down cap screw per part I did this to prevent the part from possibly twisting. The 3/8 and ¼ holes are used in the final assembly so they serve a dual purpose. It is now set up and ready to start cutting out parts.


IMG_0553.jpg


First I cut out the big chunks to minimize waste and to get them out of the way. Then made the roughing pass leaving 0.020 for final clean up. Then a clean up pass to finish. After deburing and countersinking the holes, the plates are complete.


IMG_0554.jpg


Now all of the parts are cut out and drilled. Tomorrow I’ll do the secondary operations on the parts that need it.

IMG_0555.jpg

IMG_0537.jpg IMG_0551.jpg IMG_0550.jpg IMG_0552.jpg IMG_0553.jpg IMG_0554.jpg IMG_0555.jpg
 

JimDawson

Global Moderator
Staff member
Director
Joined
Feb 8, 2014
Messages
6,458
Likes
4,436
#15
A little more progress today

The pockets in the front plate are done, just have to finish the bearing bore with the boring bar. That hole was not supposed to go all the way through, there was supposed to be a 0.109 flange left but the material vendor screwed up and delivered 7/8 thick material rather than the 1 inch I ordered and I didn't catch it, so my bad. The mark of a machinist it to be able to make a f&*^ up look like it was supposed to have been done that way. So I’ll make a nice cap for it and use that for the limit switch cam guard, nobody but us will ever know the difference.:lmao:

IMG_0558.jpg

Pocketing the motor mount. C1018 steel, 3/8 solid carbide, 2 flute, end mill. 2200 RPM spindle speed, 0.125 DOC, 5 IPM. WD-40 in the spray mist.

IMG_0560.jpg

Wading through the clearance slot in one pass. 3/8, 3 flute cobalt rougher, 900 RPM, 0.75 DOC. 0.5 IPM

IMG_0562.jpg

Finishing the bearing bore. I wanted a nice light press fit, so I bored the pocket to the bearing size –0.0002. I maybe could have done with the mill, but the boring bar is much easier to control to a fine dimension. 70 RPM, brazed carbide boring bar, 0.5 IPM down feed. This is the first boring job (there is a reason they call it boring) I have done since I did my Z-axis conversion. It’s great to be able to change both the spindle speed and the down feed on the fly. Was able to tune it right in for no chatter:thumbsup:

IMG_0564.jpg

IMG_0558.jpg IMG_0560.jpg IMG_0562.jpg IMG_0564.jpg
 

Eddyde

Active User
H-M Supporter - Sustaining Member
Joined
Oct 13, 2014
Messages
1,016
Likes
737
#16
Great work Jim, I can't understand why your client wants to us a HF press for a base, when clearly you could build a much better press from scratch. It is like putting a Rolls Royce engine in a Ford Pinto. :)
 

JimDawson

Global Moderator
Staff member
Director
Joined
Feb 8, 2014
Messages
6,458
Likes
4,436
#17
Great work Jim, I can't understand why your client wants to us a HF press for a base, when clearly you could build a much better press from scratch. It is like putting a Rolls Royce engine in a Ford Pinto. :)

Thank you for the kind words.

I tried to talk him out of it, and it would have been easier to build one from the ground up. Sometimes you just have to follow the customer's lead. When this one breaks, I'll do it my way on the next one and he can pay for it again. Job security I guess.

I had a potential customer call me yesterday and wanted to modify a 4x8 CNC wood router to a 6x12. Fortunately I was able to talk him out of that, the modification would cost more than building a gantry router from the ground up. I see building a 6x12 CNC router in my future.
 

JimDawson

Global Moderator
Staff member
Director
Joined
Feb 8, 2014
Messages
6,458
Likes
4,436
#18
I assembled the parts I have built just to check the fit. It seems to go together, but I'll have to do a bit more precision fitting.

IMG_0584.jpg
 

randyc

Active User
Active Member
Joined
Feb 5, 2015
Messages
662
Likes
553
#19
Man, I can't believe that thing will achieve 600 strokes/minute, must be punching some real thin material to be able to keep the flywheel spooled up (or maybe it doesn't have a flywheel like a conventional punch press). At ten hits per second, that HF thing is going to wear out pretty dang fast, right ?

Oh well, since your customer made some poor decisions I expect you'll get some more business from him in REPAIRS, LOL. Nice work !
 

JimDawson

Global Moderator
Staff member
Director
Joined
Feb 8, 2014
Messages
6,458
Likes
4,436
#20
Man, I can't believe that thing will achieve 600 strokes/minute, must be punching some real thin material to be able to keep the flywheel spooled up (or maybe it doesn't have a flywheel like a conventional punch press). At ten hits per second, that HF thing is going to wear out pretty dang fast, right ?

Oh well, since your customer made some poor decisions I expect you'll get some more business from him in REPAIRS, LOL. Nice work !
Thank you Randy

I had the forethought to work backward on the design. The powerhead will bolt right in to a press frame that I designed first, then adapted the mounting to the HF press. So when this one breaks, I can take the parts and install them in the new frame.

There is no flywheel, the actuating cam is direct drive from the 4200 oz-in stepper motor. The required ''tonnage'' is in the 400 lb range. I had to use a cam rather than a crank because I had to maximize the open time, I managed to get 220 degrees of on-top time and still keep the the ramps reasonable.

When I get it done, I'll try to post a video of it running. Unfortunately, I won't be able to show it with the tooling or in actual use.
 

randyc

Active User
Active Member
Joined
Feb 5, 2015
Messages
662
Likes
553
#21
Clever design and you covered your bases for the maintenance/repair issues. I sure want to see that thing in action, even without the die set !!!
 

pdentrem

Active User
Active Member
Joined
Jan 28, 2011
Messages
1,873
Likes
347
#22
Jim, interesting project.

With the advent of laser, industry is GIVING away punch presses. Why didn't the customer want to just get one of these?
Not all metals take kindly to the heat of a laser. We have been looking at laser but not 100% replacement for us. So still using presses.
 

JimDawson

Global Moderator
Staff member
Director
Joined
Feb 8, 2014
Messages
6,458
Likes
4,436
#23
OK, a little teaser for the next and last phase of the press build.

The Cam
Cam.jpg

I have a piece of a 3 inch dia. pin, what I assume is a piece of pivot pin out of an excavator bucket hinge or something like that. As you can see on the end it still has a splotch of Caterpillar yellow paint. It's hard chromed with a surface hardness of about R70C, and the depth of the hard layer is about 0.080, so it is probably induction hardened also, it is probably 415o or similar alloy. I chose this because I need a pretty tough chunk of steel for the cam

IMG_0597.jpg

I need a rough diameter of about 2.700 for final machining, so I have to remove 0.300 from the OD. Now if I had a big beefy, 10HP lathe it would be no problem, I would just take a 0.100 depth of cut and get under the hard surface in one cut, but my lathe is only a 13x40, 2 HP, so that ain't gonna happen.

So the question is how do I cut it to about 3.500 rough length, and then turn it to size using the equipment I have?

(I'll post the pictures and explanation later)
 
Last edited:

JimDawson

Global Moderator
Staff member
Director
Joined
Feb 8, 2014
Messages
6,458
Likes
4,436
#24
The cam

As I said above, this has a hard surface about 0.080 thick, but the interior is machineable. I have made a couple of parts out of this material so I knew what to expect.

No problem cutting to rough length. I have an M42 bi-metal blade in my band saw, walked right through the material, slow speed and heavy feed. No coolant so it doesn’t work harden.

IMG_0600.jpg

A test cut to figure out just how deep the hard area is. I used the brute force method of machining here. Using only the finest Harbor Freight AR-6 brazed carbide tool bit, I just started powering through the hard layer. About 0.020 DOC and 70 RPM (as slow as my lathe will turn), 0.010/rev feed. With the tool spring, it would only actually take about 0.010 DOC even though I dialed in 0.020. This was a process of taking a cut towards the chuck, then reverse the feed and let it also cut on the way back out. This presents a new cutting edge to the work. One cut, then reshapen the tool. Rinse/repeat until the hard surface is gone. I could only do half of piece at a time so once one half was done then flip it around and do the other end. The only goal here is just to get through the hard surface.

IMG_0601.jpg

Once I removed the hard layer, then I faced the end and bored the 19mm center hole to prep the work for mounting on an arbor to do the actual machining. I want all of the surfaces concentric to the bore, so this is the first operation. Many times it’s all about order of operation. On any part that requires more than one operation, I machine the whole job in my head before I ever touch the machine. I know how I’m going to hang onto the work, what tools to use, feeds and speeds. That way I don’t have to think too much while I’m actually doing the work. I can concentrate on keeping my fingers out of the spinney things.

IMG_0603.jpg

Prepping the arbor. I grabbed a chunk of 1.5 inch, 1020 shaft off of the rack to make the arbor. Normally I would not have this much stick-out for drilling the center hole because of the runout (about 0.010 at the end in this case) in the end of the shaft, but in this case I wanted the center on the lathe centerline and not in the center of the shaft. Once the turning is complete, the center will be in the center of the arbor, but not in the center of the original shaft.

IMG_0604.jpg

Using the same tool I used to remove the hard surface, I turned the arbor to size for a tight slip fit. I added a chip breaker to the tool because I hate long stringy swarf coming off the work. I need to note here that this tool bit has never seen my carbide grinder, all of the sharpening and shaping was done with a standard gray aluminum oxide grinding wheel on my bench grinder. The chip breaker was put in with the Dremel with a diamond wheel. Turning was done at 750 RPM, 0.005 feed. Tool bit just BELOW center and no nose radius, no spring back that way. As you can see the surface has a nice finish.

IMG_0606.jpg


IMG_0608.jpg

I grabbed another high quality Harbor Freight bit that I had modified for another project that was ground to about 60 degrees, I just cleaned up the grind on the bench grinder.
My old eyes don’t see as well as they used to so I put my headlamp under the tool to set the tool to the work.

IMG_0610.jpg

IMG_0611.jpg

I prefer my cross slide handle to be set at the 9:00 position, makes it easier for me to back out at the end of the cut. Since 19mm is roughly 3/4 inch, I used a ¾ -16 thread.

IMG_0612.jpg

Now the work is mounted on the arbor, and the arbor will remain in the lathe until the work is complete. I can remove the work to swap ends and maintain concentricity with the bore.

IMG_0614.jpg

Now I need to take the OD down to about 2.700 to leave enough material to generate the cam shape, and do the work on the ends for the bearing journals. This material machines really nice. 0.020 DOC, 450 RPM, 0.005 feed, using the same tool as above.

IMG_0616.jpg

More later!
 

JimDawson

Global Moderator
Staff member
Director
Joined
Feb 8, 2014
Messages
6,458
Likes
4,436
#25
Here is the cam roughed out, the bearing journals are on size but I left the one side a bit long so I would have more to grab onto for the next operation.

IMG_0617.jpg

While I was making roughing cuts I was playing with the tool height. This is where I got the best result. About 1/8 inch below center. A good finish, and no spring back. It cut exactly what I dialed in.

IMG_0621.jpg
 

JimDawson

Global Moderator
Staff member
Director
Joined
Feb 8, 2014
Messages
6,458
Likes
4,436
#27
you may need to 'splain how that happens. . .
If you are asking about running the tool below center, I may have an answer. I know it goes against everything we have been taught. I think it presents an effective positive rake on the cutting edge, and the cutting edge is better supported than running on or above center. Also as the tool wears, there is still clearance between the tool and the work rather than rubbing. Also you are cutting on the top of the tool rather than the front edge. Like a tangential tool maybe? Maybe that's the answer, not sure.

I am not totally sure about why this works but it does, and I can't argue with success. I had to make quite a few passes to turn this piece and a just kept lowering the tool on each pass until I got no spring. In this case I was making passes at about 0.030 DOC (0.060 off of the OD)

Anyone feel free to jump in here if you can explain it better.
 

randyc

Active User
Active Member
Joined
Feb 5, 2015
Messages
662
Likes
553
#28
No comment on the 1/8 below center, can't argue with success ! I'm waiting for the cam generation, LOL !
 

JimDawson

Global Moderator
Staff member
Director
Joined
Feb 8, 2014
Messages
6,458
Likes
4,436
#30
Finishing the cam

The first order of business is to make a new set of soft jaws for the mill vice. I’ve run out of places to machine on the current ones. I’m out of 1-inch aluminum so I grabbed a chunk of 7/8 x 6, C1018. I’ll use these in the vice until I chew them up so much that I need to replace them. I have a set of hard jaws, but rarely use them.

IMG_0622.jpg

Squared up, drilled and counter sunk, ready to bolt in.

IMG_0623.jpg

I put a couple of 3/8 dowel pins in to tighten against while milling the pocket

IMG_0625.jpg

Milling the pocket to fit the cam bearing journal

IMG_0626.jpg

A quick deburr with the counter sink. Same g-code, just adjusted the knee height,

IMG_0628.jpg

Ready to start machining the cam.

IMG_0629.jpg

It’s starting to look a bit cam like. I’m using a ½ inch, high-shear, aluminum cutting, 2-flute end mill. I didn’t have a 4 flute long enough to do the job. If I would have had a long rougher I would have cut the rough profile in 2 passes, but I didn’t so ya use what ya got. 3 IPM feed, 90 FPM on the spindle, 1.250 DOC, 0.020 step over per pass. About 20 passes. WD-40 in the coolant tank (the red tank).

IMG_0635.jpg

The finished profile. The surface finish came out much better than expected, that high-shear end mill did a nice job. It’s not really designed for cutting 4150. I’m surprised it lasted for the whole job; it made a lot of chips, or in this case about 1.25 long needles. Nasty little things.

The cam is a series of 3 blended arcs and one straight line. It could have been done manually on a drafting board then machined on a rotary table but it would not have been fun and would have taken a long time with several setups. I don’t know if I would have done it without a CNC. I have always designed things to be built on the tools I have available, so getting a CNC mill opened up a whole new world.

IMG_0641.jpg

And there it is on the motor shaft.

IMG_0645.jpg

I still have to put in the keyway and the set screws
 
Last edited:
[6]
[5] [7]