Getting Started with Wire EDM – How to Create Outside Features

Introduction

In this tutorial, we examine how to create Wire EDM features while learning how to use the Wire EDM Wizard. Most of the information provided can be applied to either 2 Axis or 4 Axis Wire EDM features (the differences are explained in another tutorial). A 2 Axis Outside step-by-step example is provided to explain many important concepts, and links are provided to help topics that further explain all parameters for each section.

 

This tutorial is designed to be completed first, and it should be completed with all Wire EDM Tutorials to gain a full understanding of the BobCAD-CAM Wire EDM Wizard.

Example File

The BobCAD part file for this tutorial is available for download at: http://www.bobcad.com/helpfiles. If you are connected to the Internet, you can click the link provided to download and save the Wire EDM 2 Axis Features Example 1.3dm part file. In the example file provided, the stock and machine setup are already defined for the part.

 

The part model, stock, and machine Setup for this tutorial are shown next.

 

Part 1) How to Create a 2 Axis Outside Wire EDM Feature

Add the Feature and Select Geometry

 

1. In the CAM Tree, right-click Machine Setup, and click 2 Axis Outside.
   
   The Wire 2 Axis Wizard displays.
   
   

2. In the first page of the wizard, click Select Geometry to assign the feature geometry.

 

In the graphics area, select a closed outside profile to cut. This can be wireframe geometry or the edges of a solid. The following images show both selection types for the same feature.

 

 

Tip: For 2 Axis features, you select a single profile from the top or bottom of the part. The software automatically projects the selected profile to the bottom (and top) of the stock defined for the job (2 Axis features without taper). When applying taper to a 2 Axis feature, select the profile from any Z-height and use the Taper from Bottom option to apply the taper to the bottom or top of the feature.

 

3. After selecting the profile, click (OK) to confirm the selection and return to the wizard.
   
   To learn more about selecting geometry, view the Wire EDM Wizard Geometry Selection.
   
   

4. Click Next>> to go to the Feature settings.

 

To learn about 4 Axis geometry selection, view How to Create 4 Axis Wire EDM Features.

 

Define the Feature Settings

In the Feature page of the Wire EDM Wizard, the Stock Thickness displays the height of the stock defined for the job. (This value is for informational purposes and cannot be edited in the Wire EDM Wizard.)

 

1. The Upper Guide and Lower Guide positions are positive incremental values in reference to the top and bottom (respectively) of the stock defined for the job. For this example, we use the default values.

 

Note: Most modern controllers do not require the output of coordinates from the guide positions, because they are handled at the control. In most cases, these values are only utilized for simulation purposes.

 

2. Under Glue Stop Options, confirm that Use Glue Stop with Leads is selected.
   
   When Use Glue Stop is selected, the first operation in the feature does not cut the entire profile. Instead it leaves a glue stop, defined by the Stop Distance, at the end of the chain. The glue stop is then cut using a separate Tab Cut operation. If you select No Glue Stop, then all feature operations cut the entire profile.
   
   The default Stop Distance, 0.100, is used for this feature.
   
   

3. The walls of our part are not tapered, so the Taper Setting is set to None.
   
   

4. Click Next>> to go to the Machining Strategy.

 

Define the Machining Strategy

 

1. In the Machining Strategy, select Strategy 1.
   
   This adds a Rough Cut, Skim Cut, and Tab Cut operation to the Current Operations list. Notice that because this is an outside feature, the Skim Cut operation is before the Tab Cut operation. If we performed the Tab Cut operation before the Skim Cut, our part would no longer be held in place.
   
   

2. Click Next>> to go to the Wire settings.

 

The Wire Settings

The Wire settings of the Wire EDM Wizard contains an informational display of the Wire Diameter for the job, options to create Starting Cutting Conditions, and an option to set the Rapid Feedrate used for the feature. For more information, view the Wire EDM Wizard Wire Settings and How to Create Starting Cutting Conditions.

 

1. After making any necessary changes to the Wire settings, click Next>> to go to the Posting settings.

 

Define the Posting Settings

The Posting page of the Wire EDM Wizard contains Arc/Spline Output Tolerance, or the maximum amount of variation between the selected spline, ellipse, or arc geometry and the line segments that are used to approximate them. The tolerance can be increased or decreased as needed. The Posting Order settings only apply to 2 Axis features in which you assign more than one profile to the feature. To learn more, view the Wire EDM Wizard Posting Settings.

 

1. Confirm that the proper Work Offset Number for the feature is selected.
   
   

2. Click Next>> to go to the Machine Sequence.

 

The Machine Sequence

The Machine Sequence is only used to determine the cut order when more than one profile is assigned to a 2 Axis feature. For more information, view the Wire EDM Wizard Machine Sequence.

 

1. Click Next>> to go to the Parameters of the first (Rough Cut) operation.

 

Define the Rough Cut Operation Parameters

The Standard Profile is the only pattern available for Outside features. The Compensation output for Outside features is defined as On or Off for both System Compensation and Machine Compensation in the wizard. The software automatically outputs the correct compensation codes based on your selections and the chain direction of the feature.

 

1. For this example, we use System Compensation On and Machine Compensation Off to allow the software to compensate the wire diameter based on the offset values entered in the Cutting Conditions.
   
   

2. Click Next>> to go to the Corner Types.

 

Defining the Rough Cut Operation Corner Types

The Corner Types allow you to define the type of corner output for both External Corners and Internal Corners separately for the feature. To learn more, view the Wire EDM Wizard Corner Types.

 

1. For this example, both External Corners and Internal Corners are set to Sharp.
   
   

2. Click Next>> to go to the Leads.

 

Defining the Rough Cut Operation Leads

In the Leads page of the wizard, the Start Hole Diameter of 0.00 is used because we are leading into the profile of the part from outside the stock. The Thread Vertical option is selected to force the upper and lower guides to align vertically at the start of the lead-in to the feature (the threading location). (For 2 Axis features with no taper, this option does not change the wirepath.)

 

For both the Lead-in and Lead-out of the feature, we use the default Type, Perpendicular. Because we are leading into the profile from outside the stock, we use the Perpendicular lead moves and then use the Start Point for the feature to select the desired lead-in location (after completing the wizard). We also want to make our Rough Cut lead-in longer, to come from outside the stock, and then we only need a small lead-out move for the next operation.

 

1. In the Lead-in group, in the Length box, type 0.300.
   
   This makes our lead-in start from just outside the stock.
   
   

2. In the Lead-out group, click to clear the Same as Lead-in check box.
   
   In the Length box, type 0.050.
   
   

3. Click Next>> to go to the Cutting Conditions.

 

To learn more about leads, view the Wire EDM Wizard Leads.

 

Defining the Rough Cut Operation Cutting Conditions

The Cutting Conditions page of each operation in the Wire EDM Wizard is used to add Pass Comments, define the Cutting Conditions, and define the Wire Speed and Tension for the operation. What is important to understand is that you have two ways to set the Cutting Conditions. You can either Link to Database, or you can manually enter the Cutting Conditions. When using Link to Database, the Cutting Condition parameters, Offset, Power Setting, and Feedrate, are all automatically populated from the currently selected database. The values that display here are determined using various factors from the job. The stock thickness, wire size, wire material, number of operations, and number of passes (Skim Cut operations) all determine what information is available from the database. You select the Cutting Conditions database for your machine in the Posting settings of the Current Settings dialog box.

 

Note: The Edit Table button is provided as a convenient way to set the Cutting Conditions for all operations (and passes) contained in a feature from a single location. This method should only be used when you want to manually enter the Cutting Conditions. When you change any of the three Cutting Conditions values in the Edit Table, Link to Database is automatically turned off for each operation that you edit. Changing the Tension, Speed, or Comments in the Edit Table does not turn off Link to Database. Steps are provided later in this example to show how this works.

 

1. At the top of the dialog box, notice that Link to Database is selected.
   
   Notice that all three Cutting Conditions values are unavailable.
   
   

2. Click to clear the Link to Database check box.
   
   Notice the three Cutting Conditions parameters are now available for editing.
   
   

3. Click to select the Link to Database check box. For this example we are using the database values.
   
   Notice that the Wire Speed and Tension parameters are still available. Only the three Cutting Conditions parameters can be linked to the database.
   
   

4. Click Next>> to go to the Parameters of the Skim Cut operation.

 

Define the Skim Cut Operation Parameters

The Standard Profile is the only Pattern available for Skim Cut operations.

 

1. Under Skims, select Reverse Skims.
   
   This means that the direction of each Skim Cuts pass alternates direction. (Furthermore, this means that the first Skim Cut pass cuts opposite the direction of the previous operation.)
   
   

2. In the Number of Skim Passes box, type 2.
   
   This setting means that the Skim Cut operation contains two passes, which allows for more accurate cutting and better finishing of the part.
   
   

3. Set System Compensation to On and Machine Compensation to Off.
   
   

4. Click Next>> twice to go to the Leads. (The default Corner Type, Sharp is used for External and Internal Corners.)

 

Define the Skim Cut Operation Leads

 

1. In the Lead-in group, in the Length box, type 0.050.
   
   This makes the lead-in move of the Skim Cut operation the same as the lead-out of the Rough Cut operation. Also, because the Same as Lead-in check box is selected in the Lead-out group, the lead-out uses the same settings.
   
   

2. Click Next>> to go to the Cutting Conditions.

 

Define the Skim Cut Operation Cutting Conditions

The Cutting Conditions of the Skim Cut operation are handled the same as explained in the Rough Cut operation section of this topic, with one major difference. The Selected Pass option is important when setting the Cutting Conditions for Skim Cut operations. Skim Cut operations can contain one or more passes, and the values that display in this page only apply to the currently Selected Pass. You must select each pass in the Selected Pass list in order to set the Cutting Condition for all passes contained in the operation.

 

Note: If you are not using the values from the Cutting Conditions database, you can use the Edit Table option to set the Cutting Conditions for all Skim Cut passes in a single location. Remember that changing any of the three Cutting Conditions values (Power, Offset, or Feedrate) in the Edit Table automatically turns off Link to Database for each operation that you edit.

 

The following steps are included to help you understand how to use the Edit Table.

 

1. With 2 Axis Skim Cut: Pass #1 selected in the Selected Pass list, click Edit Table.
   
   Next to 2 Axis Skim Cut: Pass #1, click in the Power Setting box, and type 782.
   
   At the bottom of the dialog box, click OK.
   
   Notice that the Link to Database check box is no longer selected. Because we edited a Cutting Conditions parameter (Offset, Power Setting, and Feedrate), the software automatically unlinks the operation from the database.
   
   

2. Click to select the Link to Database check box.
   Notice that the Cutting Conditions values are changed back to the database values.
   
   

3. Click Edit Table.

 

Next to 2 Axis Skim Cut: Pass #2, click in the Speed box and type 10, press Tab, and (in the Tension box) type 10.

 

Press Tab again (so the focus is in the Comments column), and type Comment Testing.

 

At the bottom of the dialog box, click OK.

 

Warning: The values provided (Power, Speed, Tension) in this example for the purpose of showing how to use the Cutting Conditions may or may not be appropriate values. You must confirm all Cutting Conditions are correct before running a program on your machine.

 

Notice that none of the values you just entered in the Edit Table display in the wizard. This is because the Selected Pass is still Skim Pass #1.

 

4. Under Selected Pass, click the down arrow and select 2 Axis Skim Cut: Pass #2.

 

The Wire Speed and Tension and the Pass Comment now display as entered in the Edit Table earlier.

 

Notice that the software didn’t unlink the operation from the database because none of the Cutting Conditions parameter (Offset, Power Setting, or Feedrate) were changed. The Wire Speed and Tension and the Pass Comment are not tied to the database.

 

Note: The Wire Speed and Tension are not used for all machine types. These values can be set to zero if they are not needed.

 

5. Click Next>> to go to the Tab Cut operation Parameters.

 

Define the Tab Cuts Operation Parameters

The Standard Profile is the only Pattern used for Tab Cut operations. Notice the Use Knockout parameter in the Patterns group. This parameter allows you specify a Knockout Distance, which is the length of the Glue Stop that is not cut by the Tab Cut operation. For our example we want to cut the entire Glue Stop with the Tab Cut operation, so no change is needed.

 

1. In the Compensation group, set System Compensation to On and Machine Compensation to Off.
   
   

2. Click Next>> to go to the Leads.

 

Define the Tab Cut Operation Leads

 

1. In the Lead-in group, in the Length box, type 0.050.
   
   

2. Click Next>> to go to the Cutting Conditions.

 

Define the Tab Cut Operation Cutting Conditions

Set the Cutting Conditions for the Tab Cut operation using either Link to Database, or manually enter the values after clearing the Link to Database check box.

 

Compute the Feature

 

1. At the bottom of the dialog box, click Compute to create the wirepath for the feature.

 

 

Tip: To make the wirepath easier to view, the part is made transparent (press T or click View, Transparent), and the Rough Cut operation is selected in the CAM Tree to highlight the operation.

Part 2) Select the Feature Start Point

After finishing the wizard, the feature is added to the CAM Tree below the Machine Setup. The Wire EDM Feature in the CAM Tree contains the Geometry item, which is used to modify the Start Point in addition to selecting or modifying geometry. Setting the Start Point is an important part of properly setting up your Wire EDM features. The following steps explain how to set the Start Point.

 

1. In the CAM Tree under Feature EDM 2X Outside, right-click Geometry, and click Modify Start Point.
   
   

2. In the graphics area, click the desired start point location on the feature geometry.

 

(You don’t actually have to click the geometry directly to move the start point, Modify Start Point uses the screen position of the mouse pointer, but depending on the current view, it is often easiest to click the geometry directly.)

 

 

Important: When using Modify Start Point, the geometry must be visible in the graphics area. Also, after selecting a new start point location, you must click OK to confirm the selection before computing the feature.

 

To confirm the new start point location, click (OK).

 

 

3. After modifying the start point of the feature, you must compute the wirepath to update the change.

 

In the CAM Tree, right-click Feature 2X EDM Outside, and click Compute All Toolpath.

 

 

The wirepath updates to the new start point. Notice how the first operation's lead in move is from outside the stock and all other lead moves are much shorter as explained previously.

 

To learn about modifying start points for 4 Axis features, view How to Create 4 Axis Wire EDM Features.

 

This concludes the tutorial. Be sure to view the other Wire EDM Tutorials (and help topics) using the links listed next.

Related Topics

Wire EDM Tutorials

The Wire EDM Wizard

The Wire EDM Job