The Internal Corner Cycle

Introduction

This topic will explain the Internal Corner 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 Internal Corner Cycle

 

This cycle measures the location of two perpendicular planar surface faces to determine the location of their intersection. This cycle can utilize the following geometry inputs: 

 

  • Two perpendicular lines which are aligned along the X and Y Axes.
  • Two planar surface edges which are aligned along the X and Y Axes.
  • Two planar surfaces whose normals are aligned along the X and Y Axes.

To access the Internal Corner 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

Initial Position

  • X - determines the start point for the cycle along the X-axis of the current Work Offset.

  • Y - determines the start point for the cycle along the Y-axis of the current Work Offset.

 

 

Parameters

 

  • Z Measure Height - determines the end point for the cycle along the Z-axis of the current Work Offset.

  • Corner X - defines the position of the corner along the X Axis.

  • Corner Y - defines the position of the corner along the Y Axis.

  • Update Work Offset
    - Updates the existing work offset values with the information received from the cycle.
    - Does not update the existing work offset.

 

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.

  • Two Measurements Face - specifies the face on which two contact points will be used. Choose between: 

    • Bottom Face - is the face furthest down the Y Axis.

    • Right Face - is the face furthest up the X Axis.

    • Top Face - is the face furthest up the Y Axis.

    • Left Face - is the face furthest down the X Axis.

  • First X Position - specifies the distance from the left face of the rectangle, along the X Axis, at which points of contact are to be made.
    - With this check box selected, the specified distance will be used.
    - With this check box cleared, the contact points will be automatically calculated.

  • First Y Position - specifies the distance from the bottom face of the rectangle, along the Y Axis, at which points of contact are to be made.
    - With this check box selected, the specified distance will be used.
    - With this check box cleared, the contact points will be automatically calculated.

  • Distance Between 2 Points - This cycle uses a single contact point on three sides of the rectangle, and two contact points on the other. This value specifies the distance between those 2 contact points.
    - With this check box selected, the specified distance will be used between the two points.
    - With this check box cleared, the distance between the two contact points will be automatically calculated.

Quick Steps - Internal Corner

 

  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.


  1. Update the Initial Position and Parameters sections as needed.

  2. Click the Options tab and update any options necessary.

  3. Click OK.

Example - Internal Corner

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 geometry.
  • Adjust the Initial Position.
  • Update the Parameters section.
  • 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.

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.

 

  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 the edge of the surface whose normal is parallel with the X Axis.



    The geometry is added to the Selected Geometry list, the Initial Position and Parameters section are populated, and the toolpath becomes visible.



    Since our current geometry works for a X Single Surface cycle, that is the cycle that is currently selected for us.

  3. Select the edge of the surface whose normal is parallel with the Y Axis.



    The geometry is added to the Selected Geometry list, the Initial Position and Parameters section are populated, and the toolpath becomes visible.



    Since our current geometry works for an External Corner cycle, that is the cycle that is currently selected for us.

Part 5) Updating the geometry

In this case, the geometry we have chosen could be interpreted as a External Corner cycle.Once we update the cycle, our toolpath will be on the correct side of the corner.The probing feature can do quite a bit of intelligent placement of the toolpath based on the surfaces selected.When edges are the only thing used for geometry selection, not as many assumptions can be made for the intelligent placement of the toolpath.We will take a look at how the geometry selection affects the automatic placement of the created toolpath.

 

  1. At the top of the Cycles section click the drop down list and select Internal Corner from the list.



    The toolpath and the available Parameters update.However, notice we cannot see the moves that contact the surfaces. This is due to the fact that we have only selected edges. Currently our contact points are inside of the part.Let us take a moment to correct that without having to manually update the necessary values.

  2. Next to the Selected Geometry list box, click the Delete All button.



    The geometry is removed from the list, and the edges are no longer highlighted.

  3. Select the surface whose normal is along the X Axis.



    The surface is added to the Selected Geometry list, and the toolpath updates once more showing us a X Single Surface cycle.Notice this time, the cycle is on the correct side of the surface.



  4. Select the surface whose normal is along the Y Axis.



    The surface is added to the Selected Geometry list, and the toolpath updates once more showing us the intended Internal Corner cycle.Notice this time, the cycle is on the correct side of the surface, as well as at the correct height.

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 quarter inch further forward in X.

  2. In the Initial Position group, update the Y value by adding -0.25 to the end, and pressing Tab.



    The value and the toolpath update to put the initial position further down in the Y Axis.

Part 7) Updating the Parameters section

The Parameters section for this cycle consists of the Z Measurement Height, the Corner X and Corner Y values, 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 Corner X and Corner Y values should not need to be adjusted since they are calculated automatically and list the position of the intended corner to be measured. The Update Work Offset value can be used as needed. For this example, we will skip to the Options section.

Part 8) Updating the Options section

The Options section for this cycle consist of a total of four options: X Distance, Y Distance, X Second Distance, and Y Second Distance. The X/Y Distance options allows you to set a distance from the intended corner at which the contact with the surface will be made. These distances will adjust the contact points without modifying the initial position. The X/Y Second Distance options allow you to create additional contact points on each of the surfaces. These additional contact points allow you to find the corner for surfaces that are not at a ninety degree angle. If both of the second distance options are not used, the corner is assumed to be ninety degrees.

 

  1. In the Options section, select the check box for X Distance.



    Notice the contact point updates its location along the X Axis without adjusting the initial position.

  2. In the Options section, select the check box for X Second Distance.



    Notice a new contact point is created along the X Axis.

 

Note: While the value of the X,Y Distance options define the distance from the wall, notice the value of the X,Y Second Distance determines the distance between the first and second contact points.

 

  1. In the Options section, select the check box for Y Distance.



    Notice the contact point updates its location along the Y Axis without adjusting the initial position.

  2. In the Options section, select the check box for Y Distance.



    Notice the contact point updates its location along the Y Axis without adjusting the initial position.

  3. In the Options section, select the check box for Y Second Distance.



    Notice a new contact point is created along the Y Axis. The corner is no longer assumed to be ninety degrees any longer.

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, and the probe and first move become visible.



  2. Click Next three times to view the probe movements.



  3. Click Close.

    The dialog is closed and the feature is ready to post.