Hi-helix end mills have several advantages inherited with their design.

Simple math says that a an endmill with 45 degree helix angle directs 50% of the cutting force downward versus  25% for a 30 degree end mill.

Main advantages are:

• Higher rake angle directs more of a cutting force downward.
  This reduces side load on the cutter, that leads to less deflection and less tendency to chatter.
• At high axial engagement (deeper depths of cuts) more flutes remain in the contact with the work piece. This leads to much smoother cut, again reducing tendency of the cutter to chatter.
• High helix angle pulls chips upward and away from the cutting zone.
  This reduces chip re-cutting and helps prevent cutter from getting clogged up. This also allows to take deeper cuts and increases productivity.
• Because of higher helix more of flute length is being used in the cut. Better surface finish is achieved even when using the same chip load.
  Generally an end mill with 45 degree helix can be fed 30% faster than equivalent one with 30 degree helix and still achieve same surface finish.

High helix end mills also have disadvantages that a machinist has to take into consideration:

• With more of cutting force directed axially, the load on spindle bearings in downward direction is increased.
• Tendency for both the end mill and the work piece to pull out is increased. So a more rigid tool holding and work clamping should be considered.
• Higher helix end mills are also less stiff that regular helix end mills. This may cause more deflection and may become a problem when having to machine straight walls.
  This effect should be mostly diminished by lower side radial load, but it still needs to be considered in some cases.

Just decided to store here the quotes that i liked.

And those that made me think about purpouse of life and Univerce.

The ONLY FREE CNC Speeds and Feeds Calcualtor

Confidently calculate cutting conditions for hundreds of work-piece materials and of combinations of tooling types and coatings.

• Accurately Estimate cutting forces involved in machining process and prevent tool breakage.
• Estimate machine power requirement and help choose best tool for the job.
• Suggest safe and practical Axial and Radial engagement values.
• Compensate for reduced-shank, long and extra-long tools.
• Improve cycle times and tool life
• UNIQUE feature that allows to set comfortable levels of cutter torque and deflection and prevent cutter breakage.
• Ideal for use as your Dynamic / Thoroidal / Truemill calculator

Please visit the project page for download link, support and instructions.
http://zero-divide.net/index.php?page=FSWizard_SA

If you cant, then dont clamp it at all!.
Skin it!

In here i have to program and machine several sets of roundish aluminum pieces with +/-0.001" outside tolerance. and within 0.002" thickness repeatability.
Instead if fixturing it one by one i decided to skim cut a 33" x 23" x5/8" to within 0.0015 flat. And then machine each piece completely leaving .005" outside to holt everything together.

Worked out great. 

for pics

Needed to do alot of side drilling/milling/tapping on our moulds lately.

So I quickly designed and whipped up this custom indexing fixture that allows me to mount almost anything to it.

Face plate has several tooling dowel holes on front side to locate work piece.
On the back of face plate there are 36 3/8 dia reamed holes spaced 10 Degree apart.

Housing has a big 5.0"Dia pocket in the front into which the face plate's hub fits in with 0.001" clearance
Housing also has corresponding 3/8dia reamed holes spaced apart 9 degrees. This allows me to index the face plate with 1 degree increment.

Design time:2 hours, Machining time: 2 hours.

Pictures are here:

Back View: Shows 3/8 reamed holes spaced 9 degrees apart.

Side View with mold mounted with 2 3/8-16 screws

Side View with already drilled holes

Fow Windows XP and later.

It has just been released.

Please test it out and tell me what you think!!!!!

Download it HERE http://zero-divide.net/index.php?page=FSWizard_SA

Here i will show you how to calculate Tool Engagement Angle using tool diameter and Width Of Cut (radial deopth of cut)

Lets first draw a pretty image that shows us everything we need.

Where:

• r: Radius of the cutter = Diamater /2
• a: TEA - Enagagement angle we are trying to find here
• WOC: Width of cut or RADIAL Depth of Cut
• r2: The difference between r and WOC, r=r2+WOC

Below we develop 2 formulas that allow us to find TEA and WOC

Task 1: Find WOC (Radial Depth of Cut) knowing tool engagement angle and diameter of the tool

Solution:

WOC=r-r2

r2=COS(a) * r

COS(a)=r2 / r

r2=COS(a) * R

or if we move Diameter/2 outside of brackets:

or if we replace Diameter/2 with radius:

WOC=r * (1-COS(a))

Task 2: Find engagement angle knowing WOC (Radial Depth of Cut) and diameter of the tool

Solution:

WOC =  r - r2

r2 = COS(a) * r

COS(a)= r2 / r

a = COS-1( r2 / r )

a = COS-1( ( r - WOC) / r )

a = COS-1( 1 - WOC / r )

or

a = COS-1( 1 - WOC / Dia/2 )

Thats it folks

You shall be surprised but those two formulas work also for TEA bigger than 90 Degree

Tired of printing out Operation lists and then wasting time adding setup information by hand?

There is a neat and easy way to replace standard Operations and Tooling lists with something very compact and usable.

Here are config files i use at my work to create Setup Sheets and tooling lists right from SurfCam.

1. First make sure you backup you Operations.cfg and Tooling.cfg files in case you want to go back (VERY NOT likely)
   Those can be found inside your V5 or V6\Config directory.
2. Unpack contents of the attached ZIP folder.
3. Copy .CFG files found within into your V5 or V6\Config folder.
4. Copy folder "images" into "C:\Surfcam" directory, if you want also tool images to show with tooling list.
5. Go to SurfCam Options and in section Setup Sheet select "Current" from several other choises.

Thats it!!

UPDATE!!!!!!

• Operations list NOW highlights table rows when you move the mouse over them.
• When you select ANY text on Operations List, the same text will be highlighted over the whole page!!!

Download current file below

Samples are below:

<--operations list--="">

CNC PROGRAM INFORMATION SHEET

Surfcam_custom_operations_cfg.zip Size:0.11 MB

Using Peck Cycle is often needed when drilling deep holes.
When using proper feed and speed no peck is required at depths of up to 3xDia for regular or 5xDia for High-Performance Parabolic drills.
At depths up to 10x, up to 5 pecks are required for regular  drills and up to 3 for Parabolic.
Anything over 10x Dia requires constant pecking of 0.5-1x Dia for regular drills and 1.5-2 Dia for Parabolic.

Since for programming you need a peck amount. Here are the numbers:

Of course our HSMAdvisor Speed and Feed Calculator suggests not only the Speeds and Feeds but also the proper peck depth for various drill types and depths of the hole.
It in fact was the first machinist calculator to do so. This feature was much later borrowed by our competition.

And here is a pretty image showing Peck VS Hole Depth for regular twist drill:

This not only means that peck amount should be different for different styles of drills and depths of holes.
But also that peck distance should be different for different stages of drilling the same hole.
Ideally we should start the hole with large pecks, that continually reduce as the hole gets deeper and deeper.

Let's find out how we can apply this knowledge when programming our toolpaths.
This is format for normal Pecking:

 Many machine manufacturers have variable peck drilling cycle.
This allows programmer to use deep pecks in the top of the hole and shallow pecks at the bottom.

Using this feature prolongs tool life and greatly reduces cycle time, this also makes programming proper peck easier.

Format for Variable Pecking

The sample code above was posted with Surfcam's MPost processor.
Here is the nessesary modifications to the cycle

Using this modification programmer only needs to program a single peck value and the post will automatically calculate the I and J values.

Regardless of how you get the variable pecking set up in your post, you should definitely make sure you are using this feature. As this allows you to make sure you don't only get the proper peck for the depth, but also that is is done as efficiently as possible.

In my particular case drilling thousands of deep holes in large moulds time savings were between 50% and 70% versus the regular pecking cycle.

Here are some Okuma Captain 1200 program samples for work with live tooling.
Samples are quite big so READ full article