Feeds & Speeds Tab, TURN Module

<< Click to Display Table of Contents >>

Navigation:  TURN Module > Creating Machining Operations >

Feeds & Speeds Tab, TURN Module

TURN Module allows setting of feeds and speeds to be used in the toolpaths via the Feeds/Speeds dialog. This dialog gives you the ability to set the following parameters:

 

tog_minusDialog Box: Feeds & Speeds for Turning operations
Dialog Box: Feeds & Speeds for Turning operations

Dialog Box: Feeds & Speeds for Turning operations
tog_minusDialog Box: Feeds & Speeds for Hole Machining operations
Dialog Box: Feeds & Speeds for Hole Machining operations

Dialog Box: Feeds & Speeds for Hole Machining operations
tog_minusSpindle Parameters

Constant Surface Speed (CSS)

This is the Spindle Speed Mode.  If this box is checked, the mode is set to Constant Surface Speed (CSS).  If unchecked, the mode is set to Constant Rotational Speed (CRS).
If the Constant Surface Speed is checked, the controller would automatically calculate and adjust the spindle speed based on the current diameter of the work-piece. If this calculated spindle speed is greater than the maximum spindle speed specified in your post, the spindle speed would be reduced to the maximum speed.  Refer to the Spindle section of the Post-Processor Generator to ensure your Spindle Mode is set correctly.

Spindle Speed  

his is the rotational speed of the spindle expressed in RPM.

Surface Speed  

Surface speed is set in units/min when Constant Surface Speed is selected. This is only applicable for turning inserts.

Max Speed  

The maximum rotational speed of the spindle, in RPM. This is only applicable for turning inserts.

Direction  

This determines the direction of spindle rotation and can be set to Clockwise or Counter Clockwise.
tog_minusFeed Rates

Feedrate can be set in Units/Min or Units/Revolution for Turning Inserts.

Plunge (Pf)  

This rate is the feed before the tool starts to engage in material. This is always vertical.

Approach (Af)  

This is the feedrate used that prepares the cutter just before it starts engaging into material as it starts cutting. The approach motions are dependent on the method of machining.

Engage (Ef)  

This is the feedrate used when the tool is performing an engage move. TURN Module sets this value to be 75% of the cutting speed.

Cut (Cf)  

This is the feedrate used when the tool is cutting material

Retract (Rf)  

The feedrate used when the tool is performing a retract move away from material. TURN Module sets this also to also be 75% of the cutting speed.

Departure (Df)  

The feedrate used to retract the tool from the material.

Transfer (Tf)  

This is the feedrate (in Units/Min), used for Transfer motions.  Select Use Rapid to set this to the Transfer Feed value defined in the Feeds & Speeds section of the CAM Preferences dialog.
tog_minusCoolant

Here you can override the Coolant that is specified by the Tool. Coolant can be set to Flood, Mist, Through or Air. Coolant codes are defined in the post processor generator under Misc tab. Coolant Off is also supported as a variable that can be added where needed using the post-processor generator.

Coolant selections available

Coolant selections available
tog_minusFeed Rates Reduction Factors (Hole Operations Only)

This sets Feed Rate Reduction Factors for Plunge Between Levels and the First XY pass.
tog_minusLoad from Tool

Feeds & Speeds are defined when a tool is created using Create/Edit Tools from the Machining Objects Browser.  Selecting this button loads the Feeds & Speeds from the tool that is selected for the current machining operation.
tog_minusLoad from File

This loads the Feeds & Speeds values from the Feeds & Speeds Table file.  This will display the Load Feeds from Table dialog box to make your selections.

 

Selecting OK from this dialog transfers the spindle speed and cut feedrate to the Feeds & Speeds tab. The plunge, approach, engage, retract and departure feeds are determined using a percent of the cut feed.  The percent to use for transferring the computed cut feed can be set under Feeds & Speeds Preferences.

Dialog Box: Load Feeds from Table

Dialog Box: Load Feeds from Table

Stock Material

Selecting a Stock Material and Tool Material displays the Surface Speed and Feed/Tooth. This information is contained in a feeds and speeds data file which can be edited to add newer materials.

Tool Material

Selecting a Stock Material and Tool Material displays the Surface Speed and Feed/Tooth. This information is contained in a feeds and speeds data file which can be edited to add newer materials.

Surface Speed

Selecting a Stock Material and Tool Material displays the Surface Speed and Feed/Tooth. This information is contained in a feeds and speeds data file which can be edited to add newer materials.

Feed/Tooth

Selecting a Stock Material and Tool Material displays the Surface Speed and Feed/Tooth. This information is contained in a feeds and speeds data file which can be edited to add newer materials.

The input variables - Work Diameter is automatically loaded from the Stock Radius.  Based on this parameter and the Variables Limits parameters, the program computes Spindle Speed and Cut Feedrate (Cf). measured in Unites/Revolution.  Changing the spindle speed modifies the cut feedrate.

Here you can set the Max Spindle Speed and Max Cut Feed (Cf) values.  Once these two values are set, the Spindle Speed and Cut Feed calculated by this dialog will not exceed these values even if you attempt to enter higher values into the Computed Variables fields.  To exceed these values, change them here or you must edit the operation or tool parameters manually.

The variables for Spindle Speed and Cut Feed (Cf) are computed for you based on the selections made in this dialog but will not exceed the values set in the Maximum Limits for Computation section of the dialog.  These values are then assigned to the active toolpath operation or tool.  You can override either of these variables and the other will update automatically.  Since this dialog is a Feeds & Speeds Calculator, you cannot override both values.  To do so, you must edit the operation or tool parameters manually.
tog_minusCustomizing Feeds & Speeds

TURN Module allows you to customize the feeds and speeds based on the stock material being machined, the material of the cutter employed and also the operation type. This is done by archiving your desired feeds and speeds settings in an external data file.

A default implementation of this table has been included with the VisualCAM product and can be found in a folder called "Materials" under the product installation directory.

This xml contains the list of materials, texture, feeds and speeds. The file is located under Materials folder in VisualCAM. (C:\ProgramData\MecSoft Corporation\VisualCAM 20xx\Materials).

The Materials folder contains the following files

•FeedsSpeedsDataINCH.xml  

•FeedsSpeedsDataMM.xml  

The Feeds and speeds file is an .xml file format, which can be edited using any text editor to add newer materials.

These values can then be recalled at any time to compute the feeds/speeds to be used in the current program. The format for this file is shown below.

The format for this file is shown below:

feeds-and-speeds-xml-file-format

An example entry is shown below:

feeds-and-speeds-xml-file-format-example

Note!If part unit is set to Inches, TURN Module automatically loads FeedsSpeedsDataINCH.xml and when part unit is set to MM, FeedsSpeedsDataMM.xml is loaded.