Search for tool geometry returned 2 results.

Entering Cutting Tool Geometry

September 23, 2014, 8:09 pm by admin

 

Enter Your cutting tool geometry starting with Tool Diameter (Turn diameter for Lathe)
All input fields displayed on the screen are important.

Normally when you change the tool type, default data is loaded from the database.
You can override this behavior in the Settings tab on the Fields and Limits that Reset to Default when Tool Type Changes panel by un-checking Reset Tool Data checkbox

Here are the input fields available for Tool Geometry

  • Tip Dia (Mill, Drill)

    The diameter of the cutting end of the end mill, drill, reamer etc

  • Turn Dia (Lathe)

    The diameter of the finished workpiece.

    When working in CSS and IPR mode it makes sense to keep Turn Dia equal to the actual maximum diameter of the workpiece. If you fail to do so, you may overload the spindle by calculating incorrect depth of cut and feed rate

  • N# of Flutes (Mill, Drill)

    An effective number of cutting teeth on your milling or drilling tool.

  • N# of Inserts (Lathe, Boring Bar)

    Effective number of cutting edges that do work at the same time. IE: some boring bars have 2 inserts

  • Tool Stickout

    The distance from the nose of a tool holder to the tip of the cutting tool.

    For integrated or arbor-mounted tooling, use the distance from the spindle nose to the tip of the tool.

  • Corner Radius

    Corner Radius of the insert or the tip of the tool

  • Flute Length
    Length of the cutting portion of the tool.
    Be careful as some tool types like button cutters do not allow full-depth cuts.

  • Lead Angle of the cutting edge.
    The angle between the cutting edge and a plane perpendicular to the centerline of the tool

    Common values for end mills

    90: regular straight edge
    45: Common angle for face cutters
    5-30: High feed mills

    Lower angles allow increased feed rates

  • Shank Dia
    The diameter of the non-cutting portion of the tool

  • Helix Angle
    The helix angle of the flutes.

  • Shoulder Length
    The distance from the tip of the tool to the shank of the tool. It is often the same length as the Flute Length but is sometimes larger on necked tools.

  • Tapered Shoulder
    Controls how the shoulder portion is displayed and calculated. If it is checked, the shoulder is tapered from the end of the flutes to the beginning of the shank portion.

  • Shoulder Diameter
    The diameter of the tool shoulder. It is often the same size as the Tip Diameter but is sometimes smaller for necked tools such as T-Slot cutters.

This is how the Tool Data Panel looks like for any End Mill Tool Type

Lines have been drawn to show which fields affect which tool features.

Drilling Tool Type Tool Data Panel



Turning Tool Type Tool Data Panel



Tap Tool type Tool Data Panel



Reamer, Counter Bore and Thread Mill Tool Type Tool Data Panel



See Also

 

Balancing Cutter Engagement

September 23, 2014, 10:31 pm by admin

One of the handiest functions of HSMAdvisor is the ability to suggest Depth of Cut (DOC) and Width of Cut (WOC) based on tool type and user-specified tool geometry.

When Cut data matches the default or ideal data specific for the selected Tool Type, the DOC and WOC fields turn Green in color:

This article describes how to balance the Cutter Engagement and find the most efficient way of removing material.

Case 1: Balancing DOC against changed WOC or vise-verse (Load Balancing)

Let's use the previous picture and assume our cutter is a 0.5" 3 flute Generic End Mill.
Default DOC and WOC for that kind of tool would look like this: DOC=1.0", WOC=0.150"

Set 1:
 

Now these cutting parameters are taken form the internal data base and consider Tool Type, Material being cut and even Tool Geometry.
Green color of the fields indicate that these values are ideal according to HSMAdvisor.

Let's now change the Width of Cut to full width as if we are slotting or pocketing: set WOC= 0.5"

Set 2:

As you can see default Depth of Cut (DOC) immediately changed its value and is now showing just 0.351" DOC instead of the previous 1.0"

This is it! You have just balanced Depth of Cut for the new Width of Cut you will be using.

It is noteworthy that while feed rate may change between the first two Sets of values, MRR or Material Removal Rate stays virtually the same.
This is the whole point of this Balancing exercise - to automatically adjust the other value keeping the load on the cutter the same.

Case 2: Setting both DOC and WOC to custom numbers (Feed Rate Balancing)

Let's now also change our Depth of Cut to 0.5"

Set 3:

As you can see none of the fields is green now, indicating that both of our values differ from the ideal parameters.

But if both values are not ideal, where did the difference go?

The difference went to Feed Rate. In this case Feed Rate will drop from 142 ipm to 100 ipm

When Cutter Engagement exceeds recommended values, HSMAdvisor tries to compensate the difference by reducing the feed rate.

When Cutter Engagement is less than recommended, Feed Rate may be increased, depending on the workpiece material.

 

Setting both the DOC and the WOC to custom numbers, however, leads to a nasty side-effect

As you increase cutter engagement in excess of default values, HSMAdvisor tries to reduce your Chip Load (Feed Rate).

Reduction in chip load leads to rubbing and premature tool wear.

It is HIGHLY recommended to balance at least one (DOC or WOC) without resorting to Feed Rate compensation

 

Both  DOC and WOC are set to custom values. How do I balance for one of them leaving the other one the same?

Simply Click on the text label in front of the filed you want to reset to default:

After Clicking on DOC label, Depth Of Cut re-sets  to the ideal in this circumstance value.

 

See Also