Mill Standard Drilling Example

Introduction

This topic provides an example of how to create standard hole drilling features for milling jobs in BobCAD-CAM. Standard Mill Hole features are used when drilling holes that are parallel to the Z-axis of the machine. This is the most commonly utilized drilling type in BobCAD-CAM.

 

This tutorial highlights the following functionality of the BobCAD-CAM software:

  • Using the Mill Hole Wizard to easily define drilling of more than one hole size (multiple features) in the initial wizard setup
  • Using Hole Groups to drill more than one hole depth within a single hole feature
  • Controlling the clearance, rapid, and feed planes between holes
  • Using the Machining Strategy to define the types of drilling operations applied to the holes

Example File

The BobCAD part file for this tutorial is available for download at: http://bobcad.com/helpfiles. If you are connected to the Internet, you can click the link provided to download and save the Mill Standard Drilling Example 1 BBCD.zip file. After extracting the zip file, you can open the file to follow along with this example. In the example file provided, the job, stock, and machine setup are already defined.

Create a Standard Mill Hole Feature

Set the Drilling Type and Select Geometry

  1. In the CAM Tree, right-click Machine Setup and click Mill Drill Hole.

  2. In the Mill Hole Wizard, click Select Geometry.

    The Hole Geometry Selection Manager displays.

  3. Confirm that the default drilling type, Standard Drill, is selected.

 

For this example, you can select the cylindrical surface of each hole directly from the model, but to make selection easier, a separate CAD layer contains a copy of only these surfaces. (Note that the Point and Arc Usage options do not apply when selecting cylindrical surfaces.)

 

Tip: We are selecting cylindrical surfaces because this allows the software to automatically set our diameter, top of feature, and feature depth. To learn about selecting other geometry types, view the Point and Arc Usage Example.

 

  1. In the Quick Selection group, of the Home ribbon, click Pick By Layer.

  2. In the Select Layer dialog box, click Holes.

    Click OK.



  3. Click OK in the Selection Manager.

    Geometry selection is finished. Notice the hole list displays each diameter hole and its parameters. The software automatically creates a separate Mill Hole feature for each hole diameter. The Depth value for both of our hole sizes displays as Multiple. This is due to the multiple depths that are achieved in a single feature using hole groups. The hole depths can be modified in the wizard later, as needed.

  4. Click Next>> to begin defining the parameters for the first hole diameter (feature).

Define the Feature Settings for Hole Groups

The Hole Groups table is an important part of the Feature page in the Mill Hole Wizard. Each hole group represents a different hole depth, and the Hole Groups table allows you to preview, break, regroup, rename, and set the parameters for all hole groups in the feature. ClosedClick here to expand on the subject of Hole Groups.

 

 

This section explains Hole Groups and how to define their parameters in the Mill Wizards for all Mill Hole drilling features. This information applies to standard, multiaxis, and cross drilling (Mill Turn).

What is a Hole Group?

A Hole Group can be one or more holes that share three parameters: Diameter, Top of Feature, and Feature Depth. All holes that you select for a feature that share these parameters are automatically placed into a single Hole Group. Read the following section for further hole group requirements for each drilling type.

 

Standard Drilling

The following images show a standard drilling part with holes at three different levels on the model and two hole diameters. The hole groups for this part are shown with the same color.

 

 

Notice the holes that share the same diameter, top of feature, and feature depth have the same color. The software automatically creates the Hole Groups as shown after selecting all of the holes for a single drilling feature.

 

Multiaxis Drilling

In addition to the three shared parameters, multiaxis drilling groups must also share the same tool orientation (tool vector) in order to be grouped.

 

The following images show a multiaxis drilling part with two hole diameters and five different tool orientations. The hole groups for this part are shown with the same color.

 

 

Notice that even though the three larger holes on top have the same diameter, depth, and top of feature, these holes cannot be in a single hole group because they don't share the same tool orientation (tool vector). This is also true for the two sets of smaller holes on the opposing faces, except that they do create two hole groups (shown in blue and green), one for each tool vector.

 

Cross Drilling

Cross drilling hole groups require the same three shared parameters, but the exception here is that the tool orientation/rotation angle does not affect the grouping of holes as it does in multiaxis drilling.

 

The following images show a part with all cross drill style holes at various locations around the model. There are two hole diameters with holes that share the same top of feature and feature depth. The holes groups created from this part are shown with the same color.

 

Why Use Hole Groups?

Hole groups allow you to define more than one depth for drilling within a single feature. A single hole feature can have one or more hole groups so you can optimize the hole features that you create and eliminate the need for extra features. Hole groups also provide more clearance options, or Group Retracts, to handle the rapid movements between hole groups.

Modifying Hole Groups - Feature Settings

The following information explains the use of hole groups in the Feature page of all Mill Hole Wizards.

Using the Hole Groups Table

The Hole Groups section of the Feature settings provides a table for editing Hole Groups and their parameters. You can set the Top of Feature and Feature Depth by typing the values or selecting geometry. You can also break hole groups into separate groups and then regroup them as needed, for example, to modify the rapid movement between holes.

 

Important: All of the values that display in the Hole Groups table (except Number) can be editing by clicking that item in the table and typing the new value or name. The buttons next to the Hole Groups table are used with the Hole Groups that are selected in the table. When you click a Hole Group in the table, a preview of the holes displays inside the dialog box to help you visualize the parameters for that group.

 

Hole Groups
 
Number Name Top of Feature Feature Depth
1 Group 1 -1.0000 1.0000
2 Group 2 -0.5000 1.5000
3 Group 3 0.0000 2.0000
       
     
    Break Hole Group  
       
    Regroup Hole  
       
    Pick Top  
       
    Pick Bottom  
               

 

Number

Each hole group is given a number as a reference to the group in the table. This number is automatically created and cannot be edited.

 

Name

Hole groups are automatically named in sequential order with the format of name and number (Group 1). Click the name of any hole group in the table to make it available for editing. Type the new name to create a custom name for the group.

 

Top of Feature

The Top of Feature is the top of the hole as an incremental value from the Machine Setup or machining origin location. Click the Top of Feature value in the table to make it available for editing. Type the new value to set the top of feature for the hole group. After selecting a group in the list, you can use the Pick Top button to set the value using geometry selection.

 

Important: For multiaxis drilling, the Top of Feature is in reference to the selected geometry, not the machining origin. For cross drilling, the Top of Feature is a radial distance from the center of the part (or the Z-axis of the machining origin for Mill Turn jobs).

 

 

Feature Depth

The Feature Depth is the depth of the hole as a positive incremental value from the Top of Feature. You can click the value in the table to make it available for editing. Type the new value to set the Feature Depth. You can also use the Pick Bottom button to set the value using geometry selection (after selecting a group in the list). Be sure to properly set the Top of Feature before selecting the Feature Depth.

 

Tip: For cross drilling (Mill Turn), the Top of Feature and Feature Depth values are calculated as a radial distance from the rotation axis/machining origin. Selecting cylindrical surfaces allows the software to properly calculate both of these values. When using any other geometry type, if the hole extends past the center of the part, you may need to manually type the appropriate Top of Feature and/or Feature Depth value instead of using Pick Top or Pick Bottom.

 

 

Counterbore Depth

The Counterbore Depth is the depth of the larger hole for counterbore holes. This is a positive incremental value from the Top of Feature. Click the Counterbore Depth value in the table to make it available for editing. After selecting a group in the list, you can use the Pick Counterbore Depth button to set the value using geometry selection.

 

 

Break Hole Group

The Break Hole Group button breaks the selected Hole Groups into separate single-hole groups. This can only be used when there is more than one hole in the group. Each resulting hole group contains a single hole and the naming follows that of the original group in the format: previous group name, period, new group number (Group 1.1, Group 1.2).

 

Regroup Holes

The Regroup Holes button takes all selected Hole Groups from the list and makes a single hole group. The naming of the new group follows that of the hole group with the lowest number.

 

Important: In order to regroup holes, the groups that you select must share the same Top of Feature and Feature Depth. Edit these values in the table to be the same for all holes that you want to regroup before clicking Regroup Holes. Note that for multiaxis drilling, holes must also share the same tool orientation or direction vector in order to be grouped.

 

Pick Top

The Pick Top button is used to set the Top of Feature value by selecting geometry such as a point, snap point, or surface edge. Select a Hole Group in the list before clicking Pick Top, or if you don't select a group, you can set the Top of Feature for all groups.

 

 

Pick Bottom

The Pick Bottom button is used to set the Feature Depth value by selecting geometry such as a point, snap point, or surface edge. Select a Hole Group in the list before clicking Pick Bottom, or if you don't select a group, you can set the Feature Depth for all groups.

 

 

Pick Counterbore Bottom

The Pick Counterbore Bottom button is used to set the Counterbore Depth value by selecting geometry such as a point, snap point, or surface edge. Select a Hole Group in the list before clicking Pick Counterbore Bottom, or if you don't select a group, you can set the Counterbore Depth for all groups.

 

Previewing the Hole Groups

To make it easier to visualize the parameters you are defining, when you click a group in the Hole Groups table, a preview displays inside the dialog box. The preview displays each hole, the machine setup (machining origin), the feature preview (top, bottom, and diameter), and the workpiece if you have selected one for the job.

 

 

View Controls

The Hole Groups preview uses the standard mouse controls for altering the viewing position of the preview.

    • You can Rotate the view by dragging with the left mouse button in the preview window. (You can also drag with the middle mouse button.)

    • You can Pan the view by holding down Ctrl (on the keyboard) and dragging with the middle mouse button.

    • You can Zoom in or out using the scroll wheel (rolling the middle mouse button forward or backward).

 

Viewing the Workpiece

The Hole Groups preview may or may not display the part, based on whether or not you have selected a workpiece for the job. Workpiece selection is the first step of using the Stock Wizard, or it can be assigned (or removed) using the Workpiece item in the CAM Tree.

Selecting Multiple Hole Groups

The Hole Groups table allows for multiple selections using standard controls as follows.

 

Important: You can click anywhere in the row of a group to select that group in the list. When you click any value other than the number, it becomes available for editing. When adding or removing selections using modifier keys (Ctrl or Shift), select a group by clicking its row under the Number column.

 

  • Click anywhere in the row of a group to select that group.

  • Hold down the Ctrl key and click any group to add it to or remove it from the selection.

  • After selecting one group, hold the Shift key and click another group to select all groups in between the first and second selections.

  • Tip - when you have multiple groups selected in the table, you can click any other group to select it and clear the other selections.

Hole Groups - Operation Settings

When you go to the Parameters page for any drilling operation in the Mill Hole Wizards, the Hole Groups section displays the name of each Hole Group in the feature. You then select the group name before setting the effective depth, overall depth, and cycle type settings, such as pecking, for each group.

 

 

 

  1. For now, we are using the default Material Approach settings.

 

The Diameter is already properly set from the selected geometry.

 

The Parameters are also already properly set for this example.

 

  1. Under Hole Groups, click anywhere in the row of Group 1 to select it.

 

Because the group is now selected, the hole groups preview displays inside the dialog box.

 

 

 

To change the viewing orientation of the preview, drag the left or middle mouse button to rotate. To pan the preview, press and hold the Ctrl key, and drag the middle mouse button. To zoom in or out, roll the middle mouse button forward or backward.

 

  1. In the Hole Groups table, click the name Group 1, and type Low.

 

This hole group is on the lowest level of the part, and our custom naming is more descriptive than Group 1. Renaming hole groups is a great way to stay organized when there are many hole groups.

 

Tip: To edit a hole group name, top of feature, or feature depth, click the value (or name) directly in the Hole Groups table. Type the new value or name to update it. After editing any value, you can press Tab to move to the next parameter in the list, or press Enter to finish.

 

  1. Under Hole Groups, click the name Group 2.

 

 

  1. Type Mid to rename Group 2.

  2. Click the name Group 3, and type High.



    We don't make any other changes to the hole groups at this time. Remember that we selected cylindrical surfaces so the parameters for the hole groups are automatically set.

  3. Click Next>>.

Define the Machining Strategy

  1. Under Template, click the Hole machining strategy template.

    This assigns one center drill operation and one drill operation to the Current Operations list.

  2. On the lower left, click Apply to All Features.

    The software automatically creates one feature for each hole diameter as seen in the tree on the left. The second feature now uses the same Machining Strategy as the first.

  3. Click Next>> twice to go to the center drill tool data. (No changes are needed for the posting settings.)

Define the Tool Data and Operation Parameters

  1. Notice the System Tool check box is selected. For this example, we use the automatically selected system tool information, but be sure to update the tool data, machining data, and feeds and speeds as needed when creating your own programs.

  2. Click Next>>.

    Again, we use the default operation parameters, but notice there are no hole groups listed. For center drill and chamfer operations, the parameters defined here are shared across all hole groups. All other operation types allow you to define the parameters for each hole group separately.

  3. Click Next>>.

    We use System Tool information again for the drill operation, because the software automatically loads a tool with the correct diameter from the Tool Library. All of the parameters stored with the tool are automatically set in the wizard.

  4. Click Next>>.

  5. Notice the Hole Groups list. Click Low to select it.

    Under Cycle Type, click Peck.

  6. Click the group name Mid, and then select Peck.

 

Set the High group to Peck using the same process.

 

Important: Be sure to select a hole group before changing any operation parameters, and make sure to set the parameters as needed for all hole groups.

 

  1. Click Next>>.

Define the Second Feature and Compute the Toolpath

  1. In the Hole Groups table, repeat the process of selecting the group to view the preview, and then rename each group to Low, Mid, and High based on its level on the model.

    Again, the hole groups parameters are automatically set because we selected cylindrical surfaces.

  2. Click Next>>, and notice that the Hole operation template is selected from using Apply to All Features earlier.

  3. In the tree on the left, click the last Parameters item.

  4. Repeat the process as explained earlier to set all hole groups to the Peck cycle type.

  5. On the lower-right, click Compute.

 

The resulting toolpath is shown next.

 

 

 

After viewing the toolpath, we see one issue. The rapid plane, applied within hole groups, is going through the steps of the model because the holes on opposite sides of the part are in the same group. The rapid movement between hole groups is determined by the group retracts as seen in the link moves that retract up above the part. Next we modify our hole groups to alleviate the issue.

 

Edit the Feature, Break and Regroup Holes

For reference, the following image shows the current hole groups using one color for each group. Remember that each hole diameter is a single feature and we are working with two features (both are shown in the image).

 

 

 

After breaking and regrouping holes in the following steps, the hole groups are as follows (one color for each hole group). This final grouping allows us to optimize the toolpath for both features.

 

 

 

  1. In the CAM Tree, right-click the first feature name, Standard Feature Mill Hole - 0.3750, and click Edit.

 

Click the Group Retracts button under Material Approach.

 

The group retracts handle the rapid movement between hole groups, and they are currently set to a plane in Z with a height of 0.6250. This distance is in reference to the machine setup (machining origin) location, which is at the top of the part.

 

Close the Group Retracts dialog box.

 

Next we modify our hole groups so the group retracts are used when moving from one step (level) of the model to the next.

 

  1. Under Hole Groups, click anywhere in the row of the Low group to select the group and display the preview.



  2. With the Low group selected, click Break Hole Group.

    The group is separated into four single-hole groups (Low.1 through Low.4).

  3. Click anywhere in the row of group Low.1 to select it.

 

 

Press and hold the Ctrl key, and click Low.2 to add it to the current selection.

 

 

We can see that Low.2 is on the opposite side of the part so we don't want to regroup these holes.

 

Tip: You multi-select items in the Hole Groups list using the Shift and/or Ctrl keys. Hold Ctrl and click a group to add it to or remove it from the current selection. Hold Shift and click a group to select all groups between the first and second selections.

 

Hold the Ctrl key and select group Low.2 to remove it from the selection. (Click the row of Low.2 in the Number column.)

 

 

Press Ctrl and click Low.4 to add it to the selection.

 

 

We can see that Low.1 and Low.4 are on the same side of the part, so these are the two holes we want to regroup.

 

  1. With both Low.1 and Low.4 selected, click Regroup Holes.

 

Click the new group Low.1 to confirm the new grouping.

 

 

  1. There are only two holes left on the lower level, so click Low.2, then hold Ctrl and click Low.3.

 

Click Regroup Holes to create a new Low.2 group.

 

 

  1. Repeat this process of breaking and regrouping holes for the middle level (group Mid) so that each group only contains the holes that are on the same side of the part.

 

There is no need to break the High hole group.

 

Breaking group Mid results in the following groups.

 

Mid.1

Mid.2

 

Mid.3

Mid.4

 

Groups Mid.1 and Mid.4 are regrouped to create a new group, Mid.1.

 

 

Groups Mid.2 and Mid.3 are regrouped to create a new group, Mid.2.

 

 

To update the changes for this feature, click Compute.

 

Edit the Second Feature, Break and Regroup Holes

Now we break and regroup the holes for the second feature. Again, the process here is to use the Ctrl key to add and remove selections while viewing the hole groups preview, and then regrouping the holes as needed. In this section we use the Shift modifier to select multiple list items.

 

  1. Right-click the second feature name, Standard Feature Mill Hole - 0.1250, and click Edit.

  2. Under Hole Groups, click anywhere in the row of group Low to select it.

 

Press and hold Ctrl, and select group Mid.

 

With Low and Mid selected, click Break Hole Group.

 

 

  1. Select group Low.1 and observe the hole groups preview.

 

Hold Ctrl and select Low.2.

 

Group Low.2 is on the opposite side from Low.1 and we want to regroup holes that are on the same side of the part.

 

Hold Ctrl and click Low.2 to remove it from the selection.

 

Group Low.3 is also on the opposite side of the part.

 

Hold Ctrl and click Low.4 to add it to the selection.

 

We hold Ctrl and select all the low level holes that are on the same side of the part: Low.5 and Low.8.

 

  1. With Low.1, Low.4, Low.5, and Low.8 selected, click Regroup Holes.

 

Click the new Low.1 group to display the preview.

 

 

  1. Click group Low.2.

 

Press and hold the Shift key, and click group Low.7.

 

Notice that all groups from Low.2 through Low.7 are selected.

 

 

Click Regroup Holes.

 

  1. Repeat this process to regroup the mid-level holes using the same process. (Group Mid is regrouped into Mid.1 and Mid.2 as shown next.)

 

 

  1. Click Compute to update the toolpath.

 

 

The result of breaking the hole groups is an efficient toolpath for our example part that uses a minimal rapid plane within groups and only retracts above the part to move from one group to the next (group retracts).

 

 

This concludes the tutorial.