The Boss (3 Point) Cycle

Introduction

This topic will explain the Boss (3 Point) measure cycle, will describe how to access it, will explain the options found in it, and will explain how to use it with quick steps and an example.

The Boss (3 Point) Cycle

 

This cycle measures a cylinder extruded in the Z Axis with 3 points. This cycle can utilize the following geometry inputs: 

 

• An arc whose normal is parallel to the Z Axis.
• A cylindrical surface edge whose normal is parallel to the Z Axis.
• A cylindrical surface whose normal is parallel to the Z Axis.

 

Note: The probe lifts between measurements and the touch points move in towards each other along the specified angles as this cycle is meant to measure extrusions.

 

Navigation

To access the Boss (3 Point) cycle:

 

1. In the CAM Tree, locate the desired Machine Setup for the Probing cycle, right-click the Machine Setup, and select Probing.
   
   The Probing dialog launches in the Data Entry Manager.
   
   
2. Click the Operations(s) tab.
   
   
3. Click the Parameters tab.
   
   By default the Selected Geometry list is given focus to allow you to select geometry from the graphics area.
   
   
4. Select the applicable geometry.
   
   The geometry is added to the Selected Geometry list and the Initial Position and Parameters section are populated.

 

Note: Some geometry may be applicable to several cycles. In these cases the cycle that is selected based on the geometry may not be the intended cycle. In these cases, simple choose the correct cycle from the drop down list.

The Data Entry Parameters

 

Options

• Radial Clearance - determines how close to the contact surfaces the probe should travel prior to moving down in the Z Axis.
  - With this check box selected, the value entered will determine how far away from the selected surface the probe will travel before moving down to make contact.
  - With this check box cleared, no extra clearance will be added.

Quick Steps - Boss (3 Point) 

1. In the CAM Tree, locate the desired Machine Setup for the Probing cycle, right-click the Machine Setup, and select Probing.
   
   The Probing dialog launches in the Data Entry Manager.
   
   
2. Update the Material Approach and Feature Parameters as necessary.
   
   
3. Click the Operations(s) tab.
   
   
4. On the Probe page, select, or define, the Probe to be used.
   
   
5. Click the Parameters tab.
   
   By default the Selected Geometry list is given focus to allow you to select geometry from the graphics area.
   
   
6. Select the desired piece(s) of geometry.
   
   The geometry is added to the Selected Geometry list and the Initial Position and Parameters section are populated.

 

Important: The available cycles are filtered by the geometry selected. If you selected geometry and do not have the desired cycle available, remove the geometry and reselect geometry compatible with the cycle.

7. Update the Initial Position and Parameters sections as needed.
   
   
8. Click the Options tab and update any options necessary.
   
   
9. Click OK.

Example - Boss (3 Point)

In this example we:

 

• Select the Probe feature.
• Select a probe for the cycle.
• Update the Machining Data and Feed groups.
• Select the cycle.
• Update  the cycle.
• Adjust the Initial Position.
• Adjust the Parameters.
• Utilize the Options page.
• Backplot the result.

 

Part 1) Selecting the Probe feature

The first step of any Probing cycle is to create a Probing feature in the Machine Setup it is intended to be used in.

 

1. In the CAM Tree, locate the desired Machine Setup for the Probing cycle, right-click the Machine Setup, and select Probing.
   
   The Probing dialog launches in the Data Entry Manager.

 

Note: While the Material Approach and Feature Parameters are available on the initial page of the Probing dialog, those inputs do not apply to this cycle.

Part 2) Selecting the Probe

Selecting a probe can be done with the following steps, or by simply deselecting the System Tool check box and inputting the appropriate data into the required fields.

1. By default Measure is already in the Current Operations list. This will give us access to all available measure cycles in the Operation(s) tab.
   
   At the top of the dialog, click the Operation(s) tab.
   
   
2. By default the Probe page is active. In this page, click the Tool Crib button.
   
   The Tool Crib dialog launches.
   
   
3. Select your probe from the Tool Crib.
   
   
   1. If a probe has not yet been added to your Tool Crib, select the Add From Tool Library button and select one.
      
      
   2. If a probe has not yet been added to your Tool Library, select the Add button, define the probe in the Tool Parameters section, and select OK.
      
      The probe is added to the Tool Library and is automatically highlighted.
      
      
   3. Click OK.
      
      The probe is updated in the dialog.

Part 3) Updating the Machining Data and Feed groups

When selecting a tool from the Tool Crib, a tool number, and the Height and Diameter Offsets should already be correct. However, if you need to update them, you can do that in the Machining Data group. The Feed group will allow you to set a Protected Feedrate for the probe.

1. Update the Machining Data as needed: 
   
   
   1. Update the Tool Number if needed.
      
      
   2. To have the cycle update the Height and Diameter Offset, select the Override Offset button and enter the values to update the offsets to.
      
      
2. Update the Protected Feedrate in the Feed group as needed.

Part 4) Selecting the Cycle

The cycle can be selected with the drop down list under the Cycles section, but simply selecting the appropriate geometry will usually select the required cycle automatically. Since certain geometry could be applicable to several cycles, in some cases, the list will become much smaller. In this case however, there is only one cycle possible for the geometry we choose.

 

1. Click the Parameters tab.
   
   By default the Selected Geometry list is given focus to allow you to select geometry from the graphics area.
   
   
2. Select a cylindrical surface which has been extruded along the Z Axis, or the edge of that surface.
   
   
   
   The geometry is added to the Selected Geometry list, the Initial Position and Parameters section are populated, and the toolpath becomes visible.
   
   

Part 5) Updating the cycle

In this case, the geometry we have chosen could be interpreted as a Boss (4 point) cycle.Since this is not the cycle we intended to use, we will need to update the currently selected cycle.

 

1. At the top of the Cycles section click the drop down list and select Boss (3 point) from the list.
   
   
   
   The toolpath and the available Parameters update.

Part 6) Adjusting the Initial Position

There is quite a bit of logic that goes into creating the initial position for you based on the geometry, and the cycle that you choose. While the initial position does not need to be adjusted in this case, we will play with a few of the values to explore how the toolpath reacts.

 

1. In the Initial Position group, update the X value by adding +0.25 to the end, and pressing Tab.
   
   
   
   The value and the toolpath update to put the initial position of the probe a half inch further forward in X.
   
   However, notice how the end positions are tied to the initial position. Since this is obviously not what we need, we will set that value back as it was.
   
   
2. In the Initial Position group, update the X value by adding -0.25 to the end, and pressing Tab.
   
   
   
   The value and the toolpath update to put the initial position back in its original position.
   

 

Note: Since our contact points are arranged in a radial pattern, adjusting the X,Y Initial Position will not work. However, we can adjust the Z Axis.

 

3. In the Initial Position group, update the Z value to 0.375, and press Tab.
   
   
   
   The value and the toolpath update to put the initial position of the probe down further in Z.

Part 7) Updating the Parameters section

The Parameters section for this cycle consists of the Z Measurement Height, the angles on which the contact points will extend, the Diameter and the Update Work Offset value. In this case we do not really need to adjust the height at which the probe will make contact. The diameter is automatic and should not need to be adjusted, and the Update Work Offset value can be used as needed.In this part, let's just take a look at adjusting some of the angles.

 

1. In the Parameters section, update the Third Angle value to 170 and pressing tab.
   
   
   
   The angle is updated, and we now have each contact point separated equally around the boss.
   

Part 8) Updating the Options section

The Options section for this cycle consists of the Radial Clearance value only. This value will allow you to set how far past the surfaces to move before dropping down to the contact depth.

 

1. In the Options section, select the Radial Clearance check box.
   
   
   
   The toolpath is updated to reflect the default which puts the probe 0.2 inches past the contact surfaces before dropping down.
   

Part 9) Utilizing the Options page

The values in the Options page should only be utilized if you are familiar with exactly how the individual options work.

 

1. Click the Options tab.
   
   
2. Update any and all options that are needed for the cycle.
   
   
3. Click OK to exit the dialog.
   
   
   
   The dialog closes and the Probing feature is added to the CAM Tree.

Part 10) Backploting the result

The Backplot is a great way to verify the movements of any of the operations you create.

 

1. In the CAM Tree, right-click the C Measure operation in the Probing feature and click Backplot.
   
   The Backplot dialog launches.
   
   
2. Click Next three times to view the probe movements.
   
   
   
   
3. Notice we seem to have cleared the surface with our probe.Click Next until contact is made with the surface.
   
   
   
   
4. Click Close.
   
   The dialog is closed and the feature is ready to post.