Browse: Home / Shop Doc Blog

Shop Doc – Coming Up Short

By Greg Knight on May 20, 2010

Dear Shop Doc,

I’ve been struggling with part length issues on one of my Brown & Sharpe #2 Ultramatics. The variance does not appear to be related to tool movement or collet tension as the length varies, sometimes it’s long and sometimes it’s short. The tolerance is reasonable (+/- .005). I’ve checked the regular stuff; rolls, pins, feed finger tension. Do I need to design every job to feed long and face off?

Coming up short (and long)

Dear Short and Long,

The Brown & Sharpe Ultramatic should be able to hold +/- .0025 when working properly. So no, you should not need to face every part to hold .010 total. Length variance can be particularly difficult to troubleshoot. Check one item at a time. Let’s start with the most obvious but common problems.

The feed stroke should be set to over travel by .250 maximum. If not set correctly, it cannot only exacerbate other problems, it can cause variance as the bar weight changes from a full bar to two feet of bar.

Check your trip dogs next. Make sure the feed is finished before the stop is moving. This sounds basic, but if the stop indexes away just as the collet is closing there can be variation, and it can look like the feed operation is done when it’s not.

Next, check the items involved in the lead cam actuating mechanism for the turret. First, check the lead cam shaft. If there’s any perceptible movement when you take the weight off the lead cam shaft you may have worn bearings or a bad shaft. This can cause variation because the weight of the bar changes over time as the bar gets shorter. Next, check the linkage in the lead lever mechanism. There are several fulcrum points to this lever and wear here can cause variation. Finally, check the turret rack and lever. These teeth can become worn and cause length variation. This area can also become full of chips (brass and aluminum are especially pervasive), and the chip movement can cause variation. The abrasive nature of the chips can wear the teeth away and cause huge variations. Keeping this area clear of chips should be a regular maintenance item. I have seen machines where the rack teeth look like needle points.

The withdrawal cam on the adjustment plate in the back of the machine must be kept adjusted. The proper adjustment is .002 max clearance. Brown & Sharpe recommends .001. I’ve seen machines at .015 and have often wondered how they made any good parts on them.

The last thing to check is the spindle. The only thing you need to look at here are the thrust bearings. There should be little or no endplay on the spindle. Check this with an indicator on the spindle end and then manipulate the clutches back and forth (you might as well check and adjust the clutch tension while you’re at it). There should be little or no movement in the spindle. The thrust bearings can be adjusted with the nut near the back end of the spindle.

There are several models of upgrades for Brownies available commercially, all of which eliminate any variance issues resulting from the lead cam shaft, the lever and rack, or the withdrawal cam. The withdrawal cam adjustment should be a maintenance item checked regularly along with keeping chips from the rack area.

Greg Knight and George Morris
AMT Machine Systems

Greg Knight is the Vice President of Machine Tool Automation and George Morris is an Application Engineering Manager with AMT Machine Systems in Columbus, Ohio.

Posted in , , , | 2 Responses

“Twisted” while Broaching 400 Series Stainless

By Peter Bagwell on November 22, 2009

I’m using a quarter inch hexagon broach to create a quarter inch deep form in 400 series stainless steel. However, the form is twisted, somehow spiraling from one end to the other. I don’t see any type of adjustment available on the broach holder. How can I get rid of the twist?

Spinning out of Control

Dear Spin Doctor,

The solution to removing the twist from your form is easier to find when you understand the nature of the problem. The sides of the broach include a relief angle greater than the angle of the rotary broach holder so it will not interfere with the part. The broach is held in the holder at a one degree angle. The rotary broach is designed to cut a form into the part using a cutting edge with contact points that are constantly changing. The center of the cutting edge is always kept in line with the axis of the part. As the contact point continually changes, separate chips develop in each corner of the form. As these chips increase in size, pressure is absorbed by the broach tool and tool holder. This resistance against the broach holder spindle and bearings may cause the broach to drag slightly against the material being broached. The sides of the broach cannot hold it straight because they have a greater relief angle for clearance and sometimes a spiral will develop along the length (depth) of the form.

At first you may have noticed that the form appeared smaller at the bottom. What you are really seeing is the sides of the form following this spiral path. Although there may be a slight twist, the part may still be within specification. Technicians will often recommend that you broach to the high side of your tolerance for this reason.

Work piece material can also affect this condition. Some materials could be too tough or too hard for the capabilities of the tool holder. Your material (400 series stainless) is difficult to broach, and may result in poor tool life. The combination of a dulling tool and hard material increases the thrust required to broach which increases drag thus increasing the spiraling of the form. However, at this small size and form, I’m hopeful that there are a few things you can do to try to reduce or eliminate the spiral.

First of all, good broaching practice is to check your tool holder and broach to make sure they are on center. If not, re-center the tool holder. If you are using an adjustment free model, make adjustments on the machine to assure that the broach is on center with the part. It is also good to check and make sure the pre-drilled hole is on center. Next, anything you can do to reduce the pressure caused by chip accumulation will help. Check your pre-drill diameter. Can you make it larger? The recommended pre-drill for a hexagon is 1.035 times the across-the-flat dimension. The standard quarter inch broach is likely .253 inches, and the pre-drill should therefore be .261 inches. If your customer will allow it, make the pre-drilled hole larger. This will reduce the required thrust. Have you checked your speed and feed to compare them to the recommended settings? If your tool is moving too slow, the chip may not curl over as readily as is necessary and this could result in added pressure. Increase the feed rate to improve the chip flow.

Finally, if the above recommendations do not help or are not practical, reverse the direction of the spindle at half of the depth. This will drag the spiral in the opposite direction and can reduce the overall deviation by half. Hopefully, these suggestions will help you make a turn in the right direction.

Peter Bagwell
Slater Tools Inc.

Peter Bagwell is an engineer at Slater Tools Inc., which specializes in rotary broaching tools. For more information go to www.slatertools.com

Posted in | 6 Responses

Shop Doc – When to go Hydromat

By Flavio Rovertoni on March 16, 2009

Dear Shop Doc,

We are a new job shop looking to add some equipment. We are wondering whether we should invest in used rotary transfer machines like a Hydromat Legacy or stick with multi-spindles. When would we want to use a rotary transfer machine versus the traditional multi-spindle?

When to go Hydromat

Dear When to go Hydromat,

Great question. While rotary transfers and multi-spindles can produce the same parts, a good used Hydromat Legacy will cost from $80,000 to $180,000, while a used multi will cost less than half of that. So it’s important to figure out which machine suits your specific job.

The following are some important factors to consider when choosing which machine is best suited to accomplish the most productive end result. This is not limited to just the Hydromat or multi-spindle. In some cases a CNC Swiss may be a viable alternative.

Quantity of parts: Hydromats are ideal for high volumes. For jobs making less than 20,000 pieces, the multi-spindle is the right choice. This is the case even for complex parts, because with a few exceptions they are easier to retool than a Hydromat Legacy. This is because there is more open space in the machine, which makes the spindles easier to access.

Complexity of parts: For machining complex parts that are hard to hold in collets or chucks yet can be run complete by holding onto the bar in a multi-spindle machine, it makes sense to use a multi-spindle, because there is more holding surface to grip.

But Hydromats are more versatile, because they can have 10, 12 or 16 tool spindles horizontally, or up to eight vertically. For example, machining off-center holes, radial or axial, on center holes, drilling four holes radially and not all the way through, or machining an eccentric dimension on both sides of a shaft, would be easy on a Hydromat. But doing those operations on a multi-spindle would likely be quite difficult and would add significant cost because of high cycle time.

Shape and type of material: The Hydromat is more versatile for machining different material shapes than the multi-spindle because the bar remains stationary rather than rotating. For example, machining hex material on a multi-spindle machine produces an extraordinary level of noise, while on the Hydromat there is very little or no increase in noise. The type of material you are machining should not make a difference when choosing between the multi-spindle and a Hydromat, as long as the material removal is within the limit of the motors on the Hydromat.

Tolerances: In most cases both multi-spindles and Hydromats hold comparably tight tolerances. One big advantage with a Hydromat is that it can turn a part around and machine the other end with a number of features as long as there are free stations. Back-finish on multi spindles with close tolerances is more difficult but usually required on one or more operations after it is partially finished.

However, multi-spindles have an advantage when you need to make a number of recesses (grooves) with a tight concentric requirement. In this case, it is more difficult to hold on the Hydromat, especially when the grooves are larger. It is hard to beat a form and shave tool, if it is in capable hands.

It’s also important to note that a lot of shops have been successful in combining both types of equipment by pre-machining or roughing parts to a semi-finished stage on a multi-spindle and then finishing them on a Hydromat.

Hydromat Rotary Transfer Machine (Photo from Griner.com)

Posted in , , , | Leave a response

Shop Doc – Never This Rusty

By Vincent on February 25, 2009

Today’s Machining World Archives February 2009 Volume 02 Issue 05

Dear Shop Doc,

Recently a customer contacted us stating he had received several thousand pieces, all of which had rust. I’m using a water-soluble coolant for small-machined parts. The parts are machined, dropped into baskets, processed through a corncob dryer and packed for shipping. We haven’t changed the process and products for years, so why are the parts rusting now?

Never this rusty

Dear Never this rusty,
The first thing you need to do is ask yourself the following questions about your operation: Can you verify the concentration of your coolant? If the concentration dropped below the recommended level, rust could occur.

Do you use treated or softened water or is it from the municipality? Excess salt from softened water systems can create rust or high levels of chlorine from city water that may require increased coolant concentration levels.

Has your source for metal changed recently? Perhaps the metal had some surface rust present before processing.

Did the metal supplier change the mill oil he uses? Variances in mill oils can create rust. What day were the parts manufactured? Perhaps they were manufactured on Friday and sat over the weekend, prior to being dried and cleaned?

Look at your employee records and verify that the operators who typically process these parts were present on the day the rusted parts were produced. If a fill-in or temporary employee handled them that day he or she may not have followed the standard procedure.

Did you change suppliers for your cardboard boxes? Cardboard can be acidic due to the way it is manufactured. If a change in suppliers was recently made perhaps the acidity level was increased.
Has anything changed within the plant, such as positioning of fans, vents or placement of parts?
Are the parts near an area with high forklift traffic? Forklifts use propane gas as fuel and the exhaust is highly corrosive.

Did you calibrate your refractometer? To calibrate, place the water you use on the device and look through the eyepiece. The line should indicate zero. If not, adjust accordingly.

If these questions don’t reveal your problem, you can send some processed parts, a sample from the sump and a sample of the water that is used for dilution to a lab. They can evaluate the coolant for microbiological activity, tramp oils, foam, rust protection and concentration. If bacteria are present it can deteriorate thrust inhibition package.

In your specific case it’s possible that when the operator used the corncob method for drying parts he only processed them for half the standard time. After processing, the operator packaged the parts and sealed them, creating a humidity cabinet. You may be able to decipher this by looking at water stain inside the packed rusty parts. If that’s the case, you should consider posting the processing time above the machines so that every operator knows how long the parts are to be cleaned.

Mike Pelham
International Chemical Company

Posted in , , | 2 Responses

Shop Doc – Tapered Out

By Alan Earls on October 26, 2008

Today’s Machining World Archives October 2008 Volume 04 Issue 10

Dear Shop Doc,

We’re using a horizontal band saw with automatic feed. Until recently we were cutting 12L14 RD material and we had a nice, straight cut. Then we changed to cutting 6061 aluminum SQ material, and we keep getting a tapered cut. What can we do to get rid of the taper when cutting the new type of material?

Tapered Out

Dear Tapered Out,

There are a few possible contributing factors related to your question. 12L14 is a relatively hard material, so if you were sawing too fast it could have led to premature dulling of your blade. So perhaps when you started sawing 6061 aluminum; the blade was already dull. To prevent premature blade life the saw operator must use their eyes and their ears.

First, you have to look at the chips. They should be the same color as they were when you started cutting. If they’re thick to the point of turning to a blue or brown color that indicates you’re overfeeding. On the other hand, if the chips are really skinny and resemble rice kernels that indicates that you’re not using enough feed pressure. This can do additional damage, as it can actually work harden the material and eventually cause premature dulling of the blade.

Second, you must listen to the cut — the harmonics should be pleasant sounding. If it’s “screaming” during the cut, that tells me that there’s too much vibration, which will also lead to premature wearing of the blade.

The other factor that’s very critical is the coolant, or cutting fluid ratio. We recommend using a water to cutting fluid ratio of 10 to 1. Use 2 quarts of cutting fluid to every 5 gallons of water. Cutting fluid has three functions in bandsaw applications. It flushes, cools, and most importantly provides lubricity (viscosity). You need a little slickness so the chip doesn’t adhere to the gullet of the blade itself. If the cutting fluid is too weak, you’ll get the flushing and the cooling action but you won’t get the lubricity needed. That can lead to chip weld along with premature dulling of the blade. When you mix the cutting fluid, always add the fluid to the water or it won’t mix properly. Just remember the acronym O-I-L: “oil in last.” It’s the same as dressing a salad. You have to pour the oil on after the vinegar; otherwise the vinegar will just slide off.

Another thing to remember is making sure the chip brush is adjusted and working properly. The chip brush itself should not be positioned any deeper than the shallowest gullet on the blade. If you position and align the chip brush too deep, the saw blade will cut the bristles and render the chip brush useless.

Hope this solves your problem,

Al Terronez
DoALL Sawing Products

Posted in , , | Leave a response

Shop Doc – Rotational Error When Milling Hex Stock

By Brian Such on February 26, 2008

Today’s Machining World Archives February 2008 Volume 04 Issue 02

Dear Shop Doc,

Dear Shop Doc. I’m milling a slot along the length of the part on .875 aluminum hex parts with a Mitsubishi M635 controlled Citizen-Cincom C32. In the process, my hex stock sometimes has a large twist in the bar, resulting in up to 8 degrees of rotational error from the hex fat to the milled slot. What can I do to get rid of this error?

Twist and Shout

Dear Twist,
All of the Mitsubishi M635/M700 con-trolled Citizen-Cincom machines come standard with a torque sensing feature “G160” that can be used for many interesting applications such as yours. We helped a customer a while back with the exact same problem as yours. The following is what we did.

To be quick and simple for the customer, we installed a .187 ball nose end mill in an unused live tooling station. We then programmed the tool as a probe and touched it to one side of the hex; recording the position it touched (Fig-1). We then touched the other side of the hex the same way (Fig-2). With two points known, we did a macro calculation to figure the amount of error (Fig-3), and then positioned the C axis to that value. This process only added about 3 seconds to the cycle time.

See the program example below…
M5
T800(BALL-MILL-USED-AS-PIN)
M18C0 (C axis to zero)
G50W-.5905
G98G0X1.3Z2.T8
Y.35(a Y position good for checking)
G0X1.
G160Q30.X.7F10.(check Y+ side When X axis reached 30% of load stop)
#100=#5041 (record the X value on the Y+ side)
G0X1.
IF[#5041GT.75]GOTO10
#3000=1(—ERROR -CHECK PART ROTATION)
N10(CHECK-2ND-SIDE)
Y-.35(same as above but negative)
G0X1.
G160Q30.X.7F10.(check Y- side When X axis reached 30% of load stop)
#101=#5041 (record the X value on the Y- side)
G0X1.
IF[#5041GT.75]GOTO20
#3000=1(—ERROR -CHECK PART ROTATION IS TOO BIG)
N20(DO-CALC)
#102=[#100-#101]/2
#103=ATAN[#102/.35](Find the rotation error)
G0H-#103 (re-position the C axis incrementally)
G0X1.3T0
G50W.5906

Here are a few other applications you can use the “G160” for:

  • To check if a cross drill or face drill was broken.
  • To find the location of special extruded stock with a special multi-shaped ID.
  • Often it’s used to check the collet pressure on the main- or sub-spindle to confirm clamping pressure before heavy drilling/turning.
  • You can even use it for in-process gauging to set and check offsets while running.

Good luck with your problem. If you can follow these instructions these twisting problems should get under control.

Brian Such
Marubeni Citizen-Cincom Inc.,
Cust. Support Group Manager www.marucit.com

Posted in , , , | 1 Response

Shop Doc – Tool Holder

By Vincent on June 23, 2007

Todays Machining World Archives June 2007 Volume 03 Issue 06

Dear Shop Doc,

There is this tool holder in our Brown & Sharpe tool crib that is some type of turning tool. No one here has ever used it. It has two blades but no rollers or backrest. One of the more experienced guys here said it’s a rough turning tool but thought they were hard to use. Can you tell me anything about this tool?

Just Curious

Dear Curious,
Your information is partly correct. The correct name for the tool in question is a balanced turning tool, and it isn’t difficult to use. The balanced turning tool is excellent for removing large amounts of stock at maximum rates. There are three primary ways to set the blades, depending on the requirements of the manufacturing process. In all of those cases the blades cut tangentially to the stock. Some shops have gone to carbide blades allowing for increased feeds and speeds.

The first method of setup is a true “balanced turning” application. The blades are each set at the same turning diameter; each blade removes the same amount of material that is determined by the depth of cut and the feed rate. The feed rates can vary from .005” per revolution up to .01” per revolution. However, the depth of cut can range to .250” deep, allowing .500” stock removal for one pass. The full depth of cut for each blade and the feed rate determine the thickness of the chip.

The second method for rough turning is to set each tool to remove one half of the total stock that needs to be removed. One half the full depths of cut and the feed rate will determine the chip thickness in this scenario. I personally have removed up to one inch of stock in one pass with this method, using 5/8″ turning blades.

The last method is to use the two blades as a rougher and a finisher in one pass. In this case, one blade removes 80 percent of the material. The second (finish) blade is set behind the rougher by at least the thickness of the chip (feed rate), and it removes the last 20 percent of the material. Some operators will stone the finish blade to give it some drag on the material. The feed rate will determine the quality of the finish in this case.

In all cases, the tools need to be centered and relieved properly to avoid rubbing. Three to twelve degrees, depending on material type, is a good top rake. The tool holder provides the side clearance when the blades are centered properly.

These tools are not difficult to set and they allow a much greater stock removal per pass than roller box tools. The roller box tool is preferred when a tight tolerance or superior finish is required. Good luck in using your “new” old tool.

George Morris
AMT Machine Systems

Posted in , , | Leave a response

Shop Doc – Drilling a Deep Hole on a screw machine (depth of 2.250)

By Wes Szpondowski on April 6, 2006

Today’s Machining World Archives April 2006 Volume 02 Issue 04

Dear Shop Doc,

We are a relatively new screw machine job shop that has just accepted a job in which we need to drill a significantly deep hole (a depth of 2.250). We are trying to estimate how fast we can run the job, but it’s difficult because of our inexperience at drilling holes at this depth on a multi-spindle. Any thoughts?

Sincerely, In Deep


Dear In Deep,

A few years back, we got a new job that was different than the types of parts we normally make here. The part was a steel fitting (12L 14 grade) with a hole that was .160 in diameter and almost 2.250 deep – very similar to yours. It was also a very thin piece, with a .025 wall. With very little experience in extremely deep hole drilling, I had to take an educated guess on how fast we could run the job on our 1-¼” 6-spindle National Acme. Estimating such jobs can be challenging due to the fact that the heat of the steel in many grades can affect the machining by as much as 15%, in my opinion. Upon setting the job, we realized it would run no where near the run time I had previously predicted. The part was packing with chips badly and snapping drills. Also, the process was heat treating the parts, turning them brown.

With the drills set perfectly, the machine was running an hour before all the drills broke. It had been running 50% slower than I had originally quoted the job. After a few days of doing all I could to make it run better, I decided to cut a valley into my main tool slide cam, just large enough for the cam roller to drop into. Then, I used springs to pull the main tool slide back when the roller approached the valley in the cam. It worked, and about half way through drilling, the drills pulled out, and the holes were washed out with oil. Then, the drills plunged back in to finish the cut. This kept the drills from welding up with chips in the holes. I was able to speed up the machine to our original quoted run time as a result. The machine was running with a high pressure system, but I decided to stay away from the coolant fed drills because they were $170 each, a price which would make the job significantly less profitable, considering that there were 5 drills in the machine. The most expensive drills I used were $20 each, and they did a fine job. After a few weeks, I decided to order a special cam that had a triple rise, with each rise being a progressively lighter feed, and the drop off in the cam running after the second rise. I also had the cam made 10 degrees longer than a standard in order to make room for the cut away drop off section, which needed to be wide enough for the roller to drop into. We also added a broken tool detector for drills, which kept the cost of broken tooling and sorting low. The job has run well for us ever since.

Hope this helps a bit.

Wes Szpondowski
Tool Room Leader, Wyandotte Industries. Wyandotte, MI

Posted in , , , | 1 Response

Shop Doc – Holding Tolerance Machining C12L14

By Vincent on May 19, 2013

Todays Machining World July 2006 Volume 02 Issue 06

Dear Shop Doc,

I have a customer who needs me to hold a .0005 tolerance ID on a part made with C12L14. I’ve been having trouble getting the tolerance close enough on my 6 spindle Acme bar machine. I’ve been trying for days to ream it up to specs, but I’ve never had to go this close before and I’m starting to run out of patience. Are there any tricks to getting the tolerance right.

Holding Tight

There is a technique, which may help you hold your tolerance on the part, known as ballizing. It can actually give you tolerances as close as .0001-.0002. Ballizing isn’t anything new, but usually it is utilized after machining, when you have a ball that you press through a through hole to size the ID.

What you can do is this; First, ream your part the best that you can, and then afterward, silver solder a carbide ball to the end of a shank and put it in one of your open spindles–probably your fourth position spindle on a six spindle Acme. At the same time, for this to function properly as you’re sealing everything off, you will need a little hole that will go through at an angle that doesn’t interfere with the OD of the part, to let air behind their escape as you’re ballizing the part. Then run your operation. It’s just in and out, so it doesn’t limit your cycle time of making the part. You can now complete the part on the screw machine and hold a very close tolerance, usually getting better than a 10 – 6 micro inch finish on the hole.

Things to remember
The balls are made of carbide, so you will have to experiment a little bit with size because what you’re really doing is displacing material, and it will spring back. So if you would have to hold, for example, closer than .0005 tolerances, then you will need to experiment with two or three different balls to find the result you are looking for. Also, like anything, the balls are only as good as how close you ream. In other words, the reamed hole would need to be held close to keep consistency on the ball that you’re working with. They both work a little bit together. So if you had a hole that was varying .002 before you ballized it, I still think you could ballize it and hold it within .0005. If you wanted it any closer, you would probably have to ream within .001. Then, I think you would be able to hold within .0002 or better. Also, you need to make sure that you are using, the same gauging that your customer is using.

Good luck!

Henry Bradlock
St. Joe Tool Co., Bridgman, Mich.

Posted in , , , | 1 Response

  1. Pages:
  3. 1
  4. 2
  5. 3