The 5-point Rectangle Internal Cycle

Introduction

This topic will explain the 5-point Rectangle Internal 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.

The 5-point Rectangle Internal Cycle

 

This cycle measures four sides of rectangular cut, whose walls are parallel with X and Y, in order to determine the length and width. This cycle can utilize the following geometry inputs: 

 

  • Rectangular wireframe with sides parallel to the X and Y Axes.
  • Rectangular planar surface with edges parallel to the X and Y Axes.
  • Four planar surfaces whose normals are aligned along the X and Y Axes.

To access the 5-point Rectangle Internal 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.

  • Z - determines the start point for the cycle along the Z-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.

  • Length - specifies the size of the rectangle along the X Axis.

  • Width - specifies the size of the rectangle 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

  • 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 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 - 5-point Rectangle Internal

 

  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 - 5-point Rectangle Internal

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. Rotate the part in a manner that allows you to select 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 a Y Single Surface cycle, that is the cycle that is currently selected for us.

  3. Select 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 updates to show an Internal Corner cycle.



  4. Rotate the part in a manner that allows you to select the next surface whose normal is parallel with the Y Axis.



    The geometry is added to the Selected Geometry list.



  5. Select the next 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 updates to show an 5-point Rectangle Internal cycle.


Part 5) 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.

    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.

Part 6) Updating the Parameters section

The Parameters section for this cycle consists of the Z Measurement Height, the Length and Width values, and the Update Work Offset value. In this case we will make sure we do no need to adjust the height at which the probe will make contact. The Length and Width values should not need to be adjusted since they are calculated automatically from the geometry and list the size of the rectangle to be measured.

 

  1. Move into a side view, and press S on your keyboard to turn off the Shaded view.



    In this view it is easy to see that our current Z Measurement Height will not be an issue.

  2. Press S again to turn back on the Shaded view and rotate the part back to the former view.

Part 7) Updating the Options section

The Options section for this cycle consist of a total of three options: Two Measurements Face, First X Position, and Distance Between 2 Points. The Two Measurements Face option allows you to determine which side of the rectangle will use two contact points. The First X Position allows you to determine the point along the X Axis which a contact point will be used. The Distance Between 2 Points option allows you to set the space between the two contact point which occur on the same face. For this example will explore each of the options.

 

  1. Click the drop down next to Two Measurements Face, and select Top Face.



    The toolpath updates to move the two points from the Bottom Face, to the Top Face.

  2. In the Options section, select the check box for First X Position.



    The toolpath updates. Notice the contact point on the top face is now at the same position along the X Axis as the first point on the bottom face.

  3. In the Options section, update the First X Position value by adding +0.50 to the end, and pressing Tab.



    The toolpath updates. Notice we have updated the contact points on the top face, as well as the contact point on the bottom face.

    Now we have an issue with the last contact point along the X Axis. We will need to adjust the distance between those two points to force the last point away from the right face.

  4. In the Options section, select the check box for Distance Between 2 Points.

    We can now update that value.

  5. In the Options section, update the Distance Between 2 Points value by adding -0.50 to the end, and pressing Tab.



    The toolpath updates. Notice the last contact point along bottom face is now in contact with the surface.

Part 8) 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 9) 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.