View Full Version : Project: Replacement Benchmaster Mill Handwheels (Warning - long, pic heavy)

Brian H.
03-10-2015, 11:14 PM
(Cross-posted on the Yahoo benchmastermill group)

Hi Everyone,

Back in late 2009 I acquired this Benchmaster MV-1:


The machine was complete and had the often-missing pulley cover on the spindle, but it was in rough condition both cosmetically and mechanically. The Y-axis ways were scored, the paint was flaking off, and the spindle bearings were more or less shot. I originally bought it with the intent of cleaning it up and using it as-is, with some thought given to future restoration. I took the machine apart for cleaning and, for some reason, never got around to cleaning or using it. Priorities... Fast forward a couple of years: I met an individual who was interested in my mill and offered to scrape it for me; we worked out the details, the mill was transported to them, and work began.

The Problem:

In the process of stripping off the old paint and grime, we found that two of the handwheels had been broken at some point and repaired - they could have been re-used, but they would not look or feel right when the rest of the machine would be immaculate. Ordering new commercial handwheels would be easy and relatively cheap, but the factory Benchmaster handwheels are very deeply dished and similar items are not commercially available, while I liked the feel and unique appearance of the originals and wanted to keep a similar profile. We also agreed that the factory handwheels were a bit small at 4" OD, so no buying replacements off a parted-out mill. In the end, we decided that I would attempt to make new handwheels; as of today I am finally done!


You can see the obvious repair in this photo:


Not obvious until the paint was stripped off was another break in a different handwheel, in the center hub on the machine side.

The replacements would be made from cast iron just like the originals - since I had access to heavy industrial CNC equipment at work but knew (and still know) little about casting or pattern-making, I chose to cut the parts out of continuous-cast round bar. I originally intended to increase the OD only slightly, to 4.5", but my chosen material was only available in 4" and 5" sizes. Since I would have to purchase 5" material anyways, and since the material comes somewhat oversize, I elected to make the new handwheels 5.0" OD.


I wound up doing the design twice. Since I was trying to keep the new handwheels as true to the originals as possible, except for the larger OD, this meant a lot of CAD work to get the contours correct. The first model I made didn't look right so I threw it out and reworked it from scratch. You can see the first try in the picture above.

Incidentally, there are only 9 surfaces on this model that are not inclined or three-dimensionally curved in some way...

The modeling took somewhere around 30 hours to complete; once that was done, I needed to design fixtures and program the CNC operations. That was done several times! The fixture design and the CNC programs have to work in conjunction, so changing my fixture meant, in some cases, completely re-thinking how I was going to cut the part. I decided to cut the part in two operations - the first op would hold the material in soft jaws in a 6" vise, then for the second op I would machine a plate with a round cross section groove in the face to match the half of the outer rim that had been cut. A pin would come up through the center hole to help locate the part, and to provide a place to clamp the part down.


I stayed late after work and on weekends - which were sometimes the same thing - on several occasions to work on this project. I sawed the iron to size, giving me four pieces; that would give me three for my mill plus one spare. I pulled a chunk of aluminum out of the scrap pile and roughed it into a blank the same size as the cast iron; this would be a test piece that I could scrap and not feel too bad about. The iron, on the other hand, was too expensive to purchase more and any mistake could cost me a part. Once the test piece and the soft jaws were made, it was time to run the first operation.


Looks like a handwheel! My process for machining it went something like this:

(1) 9/16 drill - this drills down to just above the surface of the center hub.

(2) 1/2 end mill - the end mill drops down into the hole previously drilled and spirals outward in multiple ~.25 Z-levels to form a rough cone shape. It then cuts in a 3-axis motion up and down the inner face of each spoke, though that surface is left somewhat heavy at this point and not finished. The areas between the spokes are roughed out, the top face of the hub is cut, and the rim is roughed out.

(3) 3/8 end mill - This cuts the small 'notch' where the handle will go, and profiles the sides of the notch to a 45 angle.

(4) Slightly less than 3/8 drill - don't recall what size I actually used. This drills the hole for the handle, which will later be interpolated out with an end mill to size.

(5) 1/8 ballnose - cuts the circular groove around the hub, finishes the rim. This tool took forever to run since I was making lots of passes with small Z levels for the sake of surface finish.

(6) 3/4 OD x 1/16R convex cutter - this tool was used to run up and down the spoke faces to finish them. It also machines the area where the rim joins the spoke; this is actually a slight undercut and I could not reach it with the 1/8 ballnose.

(7) 3mm end mill - a stock item at work, I used this to finish the 3/8 hole for the handle. This was a questionable cut, as that hole lacks only .014" from breaking out on the opposite side of the rim! Unfortunately, I did not have the second operation programmed at this point and had to run all my parts through OP1 without knowing whether the hole depth was OK (the parts came out fine).

(8) 1/4 solid carbide drill - drills the center through hole. This drill proved capable of making holes to size within .0005".

Initially, this operation ran almost 3 hours - I managed to change some of the toolpath and got it down to 2.


Brian H.
03-10-2015, 11:19 PM

I struggled with this operation for several months. None of my fixture designs or programs worked quite the way I wanted to. Programming was especially difficult; as previously mentioned, there are 9 surfaces (out of several dozen) on this part that are machinable with 2.5-axis motion, everything else has to be finished with 3-axis contouring. Most of the weird surfaces are on the second side. All the spokes are tapered along their length in both width and depth, the inner and outer spoke faces are curved, the sides have draft, and everything is blended together with .25" or so fillets. Even the fillet joining the spokes to the hub has draft. It was quite a challenge to get my CAM program (CATIA, what we used at work) to make motion that would work at all in some areas, and I had particular problems where the spokes meet the rim. Regardless of what I tried, roughing the part with a 1/2 end mill left excess material in the corners that was very difficult to machine out efficiently or without manually defining dozens of passes. I finally had success with the 1/8 ballnose, using some odd settings in the automatic roughing cycle that CATIA offers.

I was at a loss, though, since I had decided to leave my job and move out of state for multiple reasons, both personal and professional. This meant I no longer had access to the machines I needed to make my parts, or the software to program them! I tried making arrangements through the student shop at the state university an hour and a half away, which I had worked in and in fact helped set up while I was a student there. Schedule conflicts and incompatible software sunk that effort. I thought about a couple of my former co-workers who had gone into business for themselves; I had not been by to see their shop yet, perhaps I could go by and work into the conversation that I needed some parts made...

They agreed! Better yet, they also used CATIA, so all of my modeling and programming effort so far was not wasted. One of their vertical mills was likely to be sitting the next week, so they suggested I come in then. Their spindles were capable of 12,000 RPM, which was good as I was running my ballnose at 10K.

I made my OP2 fixture from a piece of 1" x 10" x 10" 6061 and some 2-3/8" round 6061. I turned the center pin from a piece of 12L14, which turned out to be a bad idea:


Everything was going smoothly until I tried to install the pin. I had designed the pin to thread into the top of the fixture, which was fine, but it would only go in up to a cylindrical register just behind the thread and stop. I assumed (oops) that the mating hole was only slightly tight, and I just needed a way to apply something beyond hand torque to the pin. I decided to use my 1/8 ballnose to cut a screwdriver slot in the top of the pin, which should work - right?

Here I made my second mistake - I was too ready to start cutting and tried too hard to get the pin in, the soft 12L14 distorted and my very accurate pin was no longer so. I really should have (a) made my pin out of some better material, and (b) designed in some sort of way to apply torque to it. After removing the pin and re-machining the internal register on the fixture, I tried again; I eventually got the pin in, but the top of my pin was now torn up. I decided that making the pin shorter would not hurt anything - a couple of passes from a 1/2" end mill cleaned up the top of the pin, a bit of deburr, a G54 zero shift, and I was ready to go.

The aluminum part was first.



With step clamps placed on opposite diagonals, a 1/2" end mill roughed out the material between the spokes. I switched the clamps and the area formerly occupied by the clamps was roughed. For finishing, I removed all of the clamps and secured the part with a single 10-24 socket head cap screw into the center pin. The 1/8" ballnose went back over every single surface except near the very top - due to tool reach I had to finish some of that area with my 1/2". Here you can see the part as it is almost finished - note the end mill removing the 'stair-stepped' profile in the center of the spoke.


Pic limit, continued...

Brian H.
03-10-2015, 11:22 PM
Continued from OP2...

I was happy with the finished part, but my cycle time was almost 5 hours for this one operation! Some re-programming later, I had a more aggressive rough that should have reduced my time by about 2 hours. I never found out, as I very quickly broke my only extended-length 1/2" EM on the first cast iron part... From my previous experience with other tools, I believed that this tool (Guhring 4-flute mold and die, .02 corner radius, solid carbide) should be able to handle the toolpath I had programmed. Apparently not. I tried using one of the shop's tools, a Hanita (now Widia) Varimill, which I had heavily used at my former workplace with excellent results. Running the same program, the Varimill had no problems whatsoever! It was a much shorter tool, though, and the tool holder was not going to clear the material when the tool was down toward the bottom of the part. It was so close, another .050 in length would have probably done it - but I just didn't have enough shank on the tool to do that, I was only holding on to 5/8 of the shank length as it was. I tried a couple of local tool distributors (it's nice to live in an area with lots of industry!) and eventually bought a long 4-flute Varimill. I tried to get a generic carbide end mill - would have been half the cost or less - but it was late Friday afternoon and the places I had time to go to did not have them. I could have ordered a replacement, but I was borrowing a machine at a commercial shop and needed to get done before another job came in for that mill.

Frustration! The new Varimill chipped the end of the flutes on the first part. It sounded fine, though... wonder how long I can make it if I reduce my feed a bit? Hmm, all four parts, evidently. the Varimill needed to be cropped and sharpened afterward, but it removed maybe 30 pounds of material! I also shaved 1-1/2 hours off the cycle time, so I am down to 5-1/2 hours per part overall, not including setup.


I actually split the roughing into a separate operation. Once all my parts were roughed, it was smooth sailing from there on. I'm very happy with the way they came out! The geometry is extremely close between the original handwheel and my new ones. It's not so much a 5" handwheel that I made and put on a Benchmaster - it IS a 5" Benchmaster handwheel.


Yesterday I went back to the shop and cleaned out their machine. Even though the material I had did not 'dust' nearly as bad as most cast iron I have seen - almost like a semi-steel - running the chipped Varimill did generate some dust that formed a fine film all over the inside of the machine enclosure. I had to wipe it (nearly) all out by hand before washing down with coolant; if that dust gets into a coolant tank it sets up like portland cement and starts... fermenting? The stuff reeks and is a huge pain to clean out once that happens. Now that's all done, they're happy, I'm happy.

I'll get the new handwheels sent out this week, I am told that final assembly can commence once they arrive.


03-11-2015, 12:12 AM
Great job and writeup. Keep posting with the rest of the machine restoration. Who do you have to do the scraping, by the way?

Brian H.
03-11-2015, 12:32 AM
I have literally been sworn to secrecy. :) The individual in question values their privacy - If I were to 'out' them on a forum, they would flatly refuse to do any further work for me! Suffice it to say that they are a master craftsman who does things as they should be done, even if that requires a fair amount of extra work. I hope I have absorbed a bit of that ethic...