MACHINING TIPS

Function of Coolents in Machining

noreply@blogger.com (Unknown) — Mon, 10 Oct 2011 13:05:00 +0000

The Coolant performs three basic functions when used in drilling, milling, and threading applications:

to reduce the heat generated during cutting
to lubricate and reduce friction between the chip and the tool
to flush out the chips.

Coolant, which is mostly water, helps to cool the chip when it is sheared away from the work piece. It includes a small amount of oil which acts as a lubricant to improve the surface finish and evacuate cut chips from the flutes/rake surface.

Because excessive heat and friction can dull a tool, coolant helps to extend tool life. Using the recommended water/oil ratio is important. Too often, users will alter this ratio significantly in an effort to reduce cost. This can cause tool life to decrease rapidly. For example, a drill which normally yields thousand holes, may now only last for a few hundred holes.

When selecting a coolant, choose one that is suitable for both the material and the particular machining operation and follow the manufacturer’s mixing recommendations. For example, high-speed machining with carbide tools might require coolant, while tapping might require cutting oil.

S. Pradeep Kumar CMP
Kennametal Knowledge Center,
Kennametal India Limited, Bangalore.

Drill Length - Smaller the better!

noreply@blogger.com (Unknown) — Fri, 02 Sep 2011 03:34:00 +0000

Many times there is a necessity of drilling holes that have a long length. The operation becomes uneconomical and also time consuming if the diameter is small and length of the drilled hole is large e.g. crankshaft oil holes can typically be 7mm diameter X140 mm long.

Experiments have shown that managing to reduce the overall length of the drill serves two purposes,1)Cost of the drill reduces and 2) Drill is less prone to a breakage (buckling effect) at higher feeds.

Examples mentioned below will show that by redesigning the holding element or guiding elements the performance of the drill could significantly be improved.

These drills (from HSS) are also specially made for deep hole drilling application and have a parabolic flute, thicker web and a high helix angle. Gun drills are common and so also are Ejector/BTA drills for higher sizes. Now solid carbide drills with internal coolant holes that use minimum quantity lubrication are becoming quite popular.

By increasing the gun drill adaptor length The length of the drill was reduced from 600 mm to 470 mm. It worked better at 20 % higher feed rate and was also cheaper.	Guide bush was removed for this oil hole drill in differential cover and a stub drill was introduced that was cheaper by 50%.

Guide bush was redesigned by cutting a slot in the original bush and mounting a smaller bush as shown above. Drill length became 200 from the original 250 mm. It performed better and was also cheaper.

By Surendra Datar
The opinions expressed here are solely of the author and are not of the company where he works

Badly drilled holes give Poor thread quality

noreply@blogger.com (Unknown) — Fri, 02 Sep 2011 03:32:00 +0000

Incomplete threads or poor thread quality are often created by using a dull drill or a reground drill that is not perfectly concentric.

Such drills create holes that may be rough and torn or crooked and bent or oval-shaped making tapping difficult.Ensure that the drill is perfectly concentric with the cutting lips of equal length and the same angles.

Holes should never be undesized and should not be tapered since threading requires straight walls.

Ensure that the material has not shrunk after drilling resulting in smaller holes. Holes drilled on surfaces that have hardened due to high temperatures or welding cannot be threaded effectively.

By Raj Kumar Singh

Tap with a Chip Breaker

noreply@blogger.com (Unknown) — Wed, 12 Jan 2011 20:27:00 +0000

Findings that came out of tapping of a soft material for our CNG engine component (Gas Link). This was an Aluminium alloy.

Chips with and without Chip Breaker on tap

Tapping of two sizes (M6 and M10) was not possible. Roll taps failed, Imported taps failed and we were doing hand tapping till the solution was found!

This methodology will also work on any long chipping material that poses a chip management problem! One has only to fine tune for the distance (1P-1.5P)! Needless to say, a sharp wheel will be required for cutting this groove in the flute (PCD/CBN depending on the tool material)

By Surendra Datar
Tata Motors Limited
Pune

Work Hardening Effect!

noreply@blogger.com (Unknown) — Thu, 01 Jul 2010 11:08:00 +0000

It has been observed that alloy steels having high carbon percent can pose a problem of work hardening of the skin because of drills that work at high cutting parameters with emulsion as a coolant. The margins (or cylindrical land) are wide in size (see photograph 1) and these burnish/rub on the cut surface. This action in the presence of the coolant leads to work hardening.

This is particularly harmful for the subsequent finishing operations.

Tapping of connecting rod bolt hole could not be done on an HMC after a full carbide internal coolant hole drill performed the core hole drilling operation. Tapping after this operation was not economical because of very poor tool life. Various tap geometries/tap tool material could not improve the tool life. The only remedy was to introduce a low speed intermediate operation (for cutting the hard skin) that produced the final size of the pre tapped (core) hole. Thus for tapping of M12x1.25 4H/5H class tolerance, the original process of diameter 10.75 mm drilling followed by M12X1.25 mm tapping was changed to 1) Diameter 10.5 mm hole drilling 2) Diameter 10.75 mm hole milling by HSS tool and 3) M 12x1.25 mm tapping!

Almost similar were the symptoms in crankshaft (shank end) drilling and tapping. Here too, an intermediate tool for removing the hard skin restored the tool life during tapping!

In case the productivity is a prime concern then this intermediate tool can be a full carbide tool (a reamer or a hole mill) that can be used at 40 to 50% of the drilling RPM! This tool can be used without coolant (air jet will help) if the taps continue to show poor performance due to effects of skin hardness. These finishing tools have a very small supporting land (or margin, see photograph 2) that does not lead to skin hardness problem.

By Surendra Datar
Tata Motors Limited
Pune

Using a diamond dressing roll

noreply@blogger.com (Unknown) — Fri, 23 Oct 2009 17:50:00 +0000

It has been observed that performance of a roller type diamond dresser can be enhanced by a methodical reversing of the dressing roll after a pre-determined number of dressings.

When the dressing role is used, abrasives particles are getting exposed on one side (the other side remains in shadow). As soon as this side gets dulled, the performance deteriorates. By conducting this experiment we could get a much better output by reversing the roll. The unused side after reversing, gave an efficient dressing before the abrasives (diamond/CBN particles) were finally dislodged exposing new abrasive particles. This works well for a disc type roller. Reversing is easy. Depending on the thickness of the layer of the PCD/CBN material, more than one reversing may have to be carried out.

For a form type of dressing roller (as shown in the photo), symmetry is necessary. In one case the design of a form type dresser had to be changed to make it symmetrical around the mounting flange.

Same theory holds good for a CBN/PCD honing tool (extensively used for example in barrel bore honing of cylinder blocks/engine blocks). Reversing cycles are now available.

For use in the reverse direction, roller dresser will have to be dismantled from the shaft and “B” side will have to be placed towards the spindle! A form type roller dresser will therefore have to be symmetrical.

Try this and see if you get enhanced output from a diamond dressing roller.

By Surendra Datar
Tata Motors Limited
Pune

Share of business

noreply@blogger.com (Unknown) — Tue, 23 Jun 2009 18:07:00 +0000

When it comes to sourcing of a product many companies protect their interest by going for two suppliers instead of depending on one. While doing so care must be exercised to ensure that performance does not change for items like tools.

This is particularly important for 'resharpening type costly full carbide drills' with internal coolant holes. There are many players in this field. Each one makes the product as per his own standard practice. We observed that resharpening must strictly be done as per original geometry. The case presented here shows that new tools performed as per expectations whereas the performance was different after resharpening because the cutting geometry was different for these two makes.

We were using a standard programme on our CNC tool resharpening machine for grinding both the types. When we switched over to two different programmes to match the original geometry we cold restore the predetermined tool life.

Photo shows one variety with 4 facets tool point for one and Cam relieved cutting point for the other! Interchange of geometry therefore must be avoided.

DSC00011: 4 facets, higher helix on flutes
DSC00012: Cam relief, slower helix
DSC00013: Cam relieved drill point
DSC00014: 4 Facets drill point
DSC00015: 4 Facets drill point

By Surendra Datar
Tata Motors Limited
Pune

Shrinking profits? Look out for tapping and reaming of cast iron parts!

noreply@blogger.com (Unknown) — Tue, 14 Apr 2009 18:16:00 +0000

We have had a number of cases where we had to increase the size of the tool while tapping and reaming of cylinder block and cylinder heads and some other parts made from GG variety of cast iron. Fortunately for standard size taps we could go for 6H X variety which is slightly oversize tap than the standard 6H tap used for getting 6H class quality of tapped hole. Same is not the case with reamers! We had to forgo the standard reamer manufacturing tolerance of 50-85% of indicated hole tolerance and make reamers of size same as the maximum tolerance value. To give an example, for getting tappet bores of size 28H8(0 to0.033 mm) in one of our cylinder blocks we have been using a reamer with a manufacturing tolerance 28.033-0.010 !

This was done to overcome the shrinkage of part size after reaming is done. Earlier when the reamer was new the holes were within tolerance but on mid size and lower. We were not getting sufficient tool life because number of grindings (resharpenings) were getting limited. Now with the basic size higher we get sufficient number of parts with more resharpenings to make the operation economical.In a nutshell this is as goos as saying use H8 size reamer for H7 size hole!

As an interim measure it is also possible to TiN coat reamers (and build size), confirm the result and then change the tool drawing value. To meet urgency slightly undersize reamers can be coated and used .By coating the size of the tool will be marginally higher.

Same technique can be used for taps. We have a few varieties of special sizes in which the basic size of the tap is higher than standard tolerance to overcome the tendency of shrinkage (and hence lower overall tool life because we do grind taps on lead as well as flutes). In the example we are using 6H class tap for 4H quality tapping.

Since reamers are best reground between centers ( CNC machines are costly) on T&C grinder, we have many reamers with a counter bore (recessed center) to retain the center during subsequent resharpening of reamers being used for reaming of blind holes. This feature will give many more grindings on a reamer. See the attached drawing

Accidental damage can lead to increase in manufacturing cost

noreply@blogger.com (Unknown) — Sat, 14 Mar 2009 07:02:00 +0000

While dealing with transfer lines and SPM we came across a few instances where the same machine was equipped with adjustable adaptors of varying length and there was a collision of adaptor with guide bushing. This could have been averted by proper training of the user but constantly changing demands led to a different user at a different time and we had to come up with a mistake proofing idea.

This was a simple modification of the earlier setting gauge by adding a strip which checks whether for the correct setting of overall length of the drill or a similar tool the adaptor will remain clear of the guide bushing or not. With this modification, collision of adjustable adaptors with guide bushing could be completely eliminated.

Photograph of 1) tools with varying length but set to the same overall length with an adjustable adaptor and 2) A photograph of a typical setting gauge with modification for adaptor fouling check strip.

By Surendra Datar
Tata Motors Limited
Pune

Here is an idea which will help reduce the cost of machining

noreply@blogger.com (Unknown) — Mon, 05 Jan 2009 08:37:00 +0000

It might be necessary to make your own design of tool holders

In order to get the best out of tools it might be prudent to come up with own designs of tool holders.

Often the return on investment is less than a month or two!

We had a cut out milling operation in our rear axle.

Initially we were using a brazed tip end mill and then migrated to indexable tip design.

We realized that with our own design of a milling cutter the expense on buying of new inserts could be eliminated. The used tips are used on the same production line. Users now get the best of this square insert.

We could do the same for one of our rough boring operation on cylinder block crank bore/Cam bore set up on CNC machine.

Tooled up machine used the inserts with smaller included angle. We came up with our own idea to put to use the larger included angle making one of the roughing operation free of insert cost.This could be done for two different sizes of inserts getting used in large numbers.

By Surendra Datar
Tata Motors Limited
Pune

Step drill steps on the cost!

noreply@blogger.com (Unknown) — Thu, 06 Nov 2008 06:05:00 +0000

Here is an interesting finding

If in a CNC operation there is more that one step drill of the same size then using a plain drill and chamfer drill gives significant benefit.

In the time a new step drill is called, one can call for a chamfer drill and get chamfers done at a substantially lower cost

We were using two step drills for machining cylinder block of our one ton vehicle called Ace on NTC machine.
The step lengths were different but the size of small diameter was same.
There were a couple of instances of breakage at the step (may be because speed/feed were not optimum for higher size but ok for smaller size) . Also manufacturing a step drill from higher size might induce stresses at the corner

Changing to a plain drill + Chamfer drill stopped the breakage and chamfer drill can also be without coolant hole (cutting down the cost further). here are the relevant photographs + PP slides. I must mention here that this tooling had come from NTC Japan.

By Surendra Datar
Tata Motors Limited
Pune

Recycle XNAT inserts

noreply@blogger.com (Unknown) — Mon, 03 Nov 2008 11:18:00 +0000

Are you using XNAT inserts?

These go on TaeguTec finish milling cutters in the name of INNOTOOL

We have started recycling these with good results. For some areas we also TiN coat these for identification.

Both Hi-Cut and Deepnanda in Pune are supplying the recycled insert

These can be used on the periphery for critical areas and for N9 quality, both periphery and face can use recycled inserts

By Surendra Datar
Tata Motors Limited
Pune

Chip management

noreply@blogger.com (Unknown) — Mon, 08 Sep 2008 17:30:00 +0000

By Surendra Datar
Tata Motors Limited
Pune

With auto loaders chip management becomes crucial and becomes difficult if the turning gets combined with facing. Chip breaker grooves work efficiently in turning but fail in facing because the approach angle becomes very small. This small approach angle (see red color) reduces the chip thickness thus making it difficult to break the chip. Chip breaking can significantly be improved by making the approach angle larger. In CNC machines, by breaking the cycle just before facing and going back from OD to earlier turned diameter (see black color).
By carrying out this change in the programme, approach angle becomes favorable and chips break efficiently (as good as those observed in turning). Compare blue color and black. Although some seconds will be lost in so doing, there will be no need to stop the machine and remove entangled chips on supporting centre or the part. We could not do so on a copy turning lathe. We therefore cranked the holder and increased the angle. This made the chip management much better.

Taper Milling? ------No, a good flat milling! Give it a try !!

noreply@blogger.com (Unknown) — Tue, 19 Aug 2008 11:54:00 +0000

By Surendra Datar
Tata Motors Limited
Pune

Cylinder block and cylinder head contacting surfaces are demanding on quality w.r.t. flatness and surface roughness.

On CNC machines, a high price is paid for finish milling of these surfaces to get a desired quality.

On SPM this task is simple and economical primarily because of a slight tilt in spindle which helps avoid a back cut !

Following experiment has given very good result. Unfortunately, this is possible only on HMC and with CNC rotary work table. If you have it then try it yourself and see the result !

This way, back cut is eliminated, tool life increases because re-contact and rubbing is absent. Time can be saved by withdrawing the cutter as soon as leading edges are out of the part. Higher the cutter diameter, higher the benefit

CNC milling programme! Tilt the work piece by 0.03-0.05 mm and mill parallel to the tilt surface by withdrawing the cutter by the same amount by which the part is tilted !!

Do you have correct approach ?

noreply@blogger.com (Unknown) — Tue, 19 Aug 2008 11:43:00 +0000

We carry out fine boring of barrel bores of 6 cylinder and 4 cylinder engines on SPM as shown

We found that the original tooling was use of two 80 degree corners of a CCMT insert

when the consumption of these tips ran into thousand plus per year for making more than 100000 blocks we had to do something to tap the potential of the other two unused corners,

With a LH holder designed to take 100 degree corner of the throwaway tip the cost could be halved.

We then extended the scheme to cut Crank bore and Cam bore on Makino tooled up machine and got the same benefit.

Surendra Datar
Tata Motors Limited
Pune