I found the recent topics quite interesting since there are some ON
TOPIC threads going on these past few days in this newsgroup regarding
cutting tools.

So the thread on “Quiz / Quote This Job” I started leads right into a discussion coming out of the “A New Facemill” thread started by PV. So I’m joining them together to explain what my intent was with the Quiz.

First off, the answer I came up with on the Quiz was 49.7 Seconds TOTAL CUT TIME for both endmills combined to cut the flat and radius channels in the parts. That would be Answer “C”. However if the seconds were NOT rounded and extra safe positioning distances were added into the cutting path, the TOTAL CUT TIME could be debated as being over 50 seconds which would be Answer “D”. I will take either one of those answers because this is Real Life.

There are differences of opinion on how to quote any job. But the fact that a few seconds is what you would be debating on and not SEVERAL MINUTES is great in my opinion.

My math explanation will eventually result in describing the METAL SLASH MILLS seen on the Sumitomo link as well as other High Feed Milling Tools and the theory that is used to achieve the Feeds they claim are possible by using these tools properly with Low Horsepower Machines.

The Radius Channel used a ¾” Ballnose Endmill. Since the Depth of cut is not 3/8” of an inch which is the full depth of the radius on the ballnose it cannot be calculated as a ¾” ballnose, it needs to be calculated at something smaller than ¾”, The Shallow Depth of .0215” then makes the TRUE CUTTER DIAMETER approximately ¼” diameter. Now the 500 SFM for a ¼” diameter calculates to 7,630 RPM with .002 FPT and 4 flutes calculates to 61 Inches Per Minute Feedrate. Where as the standard ¾” endmill using the same SFM & FPT is running 20.333 IPM.

Each cutter begins cutting material ½ of the cutter diameter away from the part as it enters the part and continues to cut ½ of the cutter diameter past the end of the part. So the ¾” Standard endmill cuts a distance of 12-3/4” inches. The Ballnose Endmill which is truly cutting at ¼” diameter will travel 12-1/4” inches.

Standard endmill travels 12.750” divided by 20.3 IPM=.628 minutes =37.7 seconds Ballnose endmill travels 12.250” divided by 61 IPM=.200 minutes = 12 seconds Totalling 49.7 Seconds Cut time for both endmills combined.

The Point : These Two ¾” endmills should not be running the same RPM or IPM simply because they are described as ¾” endmills. The effect that the depth of cut has on the Ballnose Endmill dictates you should run them differently. In this scenario the benefits are huge savings of time and money. Not only would you save 25 seconds per part but the ballnose is now running at the proper SFM resulting in better tool life resulting in reduced tool cost.

But here is where I was taking this regarding The Metal Slash Mills. Now if you picture how the ¾” ballnose transformed into a ¼” endmill due to the shallow depth of cut, you will follow this easily.

Imagine a 20” Ballnose Cutter. (If you truly ran a cutter like this you would soon find out that your chiploads are really high, like maybe into the .025”, .035” or more due to making this monster cut and not rub is why the higher chipload would take place.) Then with this large ballnose cutter you only take a .060” Depth of Cut. This would make the TRUE CUTTING DIAMETER about 2-3/16” diameter.

Now let’s make some inserts that are somewhat standard size milling inserts but they have a form on them that would simulate a 20” ballnose form when positioned properly on the 2-3/16” diameter cutter body.

If you use this body with these inserts at the shallow depth of .060” AND AT THE PROPER CUTTING PARAMETERS you would now be cutting exactly like these High Feed Milling Cutters you see in these videos all of the time on CAT40 15HP machines. It’s not magic. It’s just doing the math properly and taking advantage of the technology to save time, which is much more costly than the tooling cost.

Search out the videos of these high feed mills. As you see what they are really up to you begin to understand the relationship it has with the QUIZ / QUOTE THIS JOB thread and my intent to make sure you are not afraid of trying these cutters out to be more profitable.

I hope this was worth the time reading. Good Luck, JR

So the thread on “Quiz / Quote This Job” I started leads right into a discussion coming out of the “A New Facemill” thread started by PV. So I’m joining them together to explain what my intent was with the Quiz.

First off, the answer I came up with on the Quiz was 49.7 Seconds TOTAL CUT TIME for both endmills combined to cut the flat and radius channels in the parts. That would be Answer “C”. However if the seconds were NOT rounded and extra safe positioning distances were added into the cutting path, the TOTAL CUT TIME could be debated as being over 50 seconds which would be Answer “D”. I will take either one of those answers because this is Real Life.

There are differences of opinion on how to quote any job. But the fact that a few seconds is what you would be debating on and not SEVERAL MINUTES is great in my opinion.

My math explanation will eventually result in describing the METAL SLASH MILLS seen on the Sumitomo link as well as other High Feed Milling Tools and the theory that is used to achieve the Feeds they claim are possible by using these tools properly with Low Horsepower Machines.

The Radius Channel used a ¾” Ballnose Endmill. Since the Depth of cut is not 3/8” of an inch which is the full depth of the radius on the ballnose it cannot be calculated as a ¾” ballnose, it needs to be calculated at something smaller than ¾”, The Shallow Depth of .0215” then makes the TRUE CUTTER DIAMETER approximately ¼” diameter. Now the 500 SFM for a ¼” diameter calculates to 7,630 RPM with .002 FPT and 4 flutes calculates to 61 Inches Per Minute Feedrate. Where as the standard ¾” endmill using the same SFM & FPT is running 20.333 IPM.

Each cutter begins cutting material ½ of the cutter diameter away from the part as it enters the part and continues to cut ½ of the cutter diameter past the end of the part. So the ¾” Standard endmill cuts a distance of 12-3/4” inches. The Ballnose Endmill which is truly cutting at ¼” diameter will travel 12-1/4” inches.

Standard endmill travels 12.750” divided by 20.3 IPM=.628 minutes =37.7 seconds Ballnose endmill travels 12.250” divided by 61 IPM=.200 minutes = 12 seconds Totalling 49.7 Seconds Cut time for both endmills combined.

The Point : These Two ¾” endmills should not be running the same RPM or IPM simply because they are described as ¾” endmills. The effect that the depth of cut has on the Ballnose Endmill dictates you should run them differently. In this scenario the benefits are huge savings of time and money. Not only would you save 25 seconds per part but the ballnose is now running at the proper SFM resulting in better tool life resulting in reduced tool cost.

But here is where I was taking this regarding The Metal Slash Mills. Now if you picture how the ¾” ballnose transformed into a ¼” endmill due to the shallow depth of cut, you will follow this easily.

Imagine a 20” Ballnose Cutter. (If you truly ran a cutter like this you would soon find out that your chiploads are really high, like maybe into the .025”, .035” or more due to making this monster cut and not rub is why the higher chipload would take place.) Then with this large ballnose cutter you only take a .060” Depth of Cut. This would make the TRUE CUTTING DIAMETER about 2-3/16” diameter.

Now let’s make some inserts that are somewhat standard size milling inserts but they have a form on them that would simulate a 20” ballnose form when positioned properly on the 2-3/16” diameter cutter body.

If you use this body with these inserts at the shallow depth of .060” AND AT THE PROPER CUTTING PARAMETERS you would now be cutting exactly like these High Feed Milling Cutters you see in these videos all of the time on CAT40 15HP machines. It’s not magic. It’s just doing the math properly and taking advantage of the technology to save time, which is much more costly than the tooling cost.

Search out the videos of these high feed mills. As you see what they are really up to you begin to understand the relationship it has with the QUIZ / QUOTE THIS JOB thread and my intent to make sure you are not afraid of trying these cutters out to be more profitable.

I hope this was worth the time reading. Good Luck, JR