Hole
Feature 
Insert
Features
Use this command to create a variety of hole
features. Simple, tapered, counterbore, countersink and spot face holes
are supported with different end type options including blind, until face
and through all. With hole features you can incorporate attributes that
can be extracted
by other VX levels (e.g., Drawing Sheet and CAM).
These attributes include threads, tolerances and call out labels. You can load and save hole attribute bundles allowing you to develop custom hole libraries. The hole preview echo will display in red if the supplied hole parameters are invalid for the given application. Refer to the options below for more information.
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Hole features should be considered final features like fillets and chamfers. Modeling efficiency is improved when these features are added later in the design. |
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You can assign hole attributes to a hole shaped region created by some non-hole feature (e.g. imported, Boolean remove a cylinder, revolve a notched profile, etc.) using the Flag Hole Feature command. |
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When creating multiple holes, a preferred practice is to pre-define a sketch with point entities at the hole locations. Right-Click and selecting the “Sketch” option will prompt you to select a sketch. You can skip this option entirely by simply selecting a sketch directly from the History Manager when prompted for hole locations..
The coordinates of point entities in the sketch will be input to the active point input list. When the history regenerates, it will pick up the points currently defined in the sketch, replacing any previous point coordinates stored with the feature. This is useful for controlling the number and placement of holes in a part using a sketch. |
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Simple Holes
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Tapered Holes
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Countersink Holes |
Counterbore Holes |
Hole type
This sets the desired hole type to Simple, Tapered, Counterbore, Countersink or Spot Face A picture of the hole type will be displayed and the appropriate input fields will be activated. Only blind holes are shown here. Other end types include Until Face and Thru-All (see below)
Face
Select the plane to place the hole feature. You can select a datum plane, planar face or a sketch.
Location
Select the hole locations and then middle-click to continue. Multiple holes can be created, but all will be considered one feature with the same dimensional characteristics.
Input Fields
Input fields are provided for entering hole dimensions. The active dimensions depend on the hole type selected above.
Dia (D1) - Primary hole diameter. For threaded holes (see Optional Inputs below), D1 refers to the tap drill diameter when using hole bundles from the Hole Standards Library (see below).
Depth (H1) - If the end option (see below) is set to Blind, specify the hole depth here.
D2 - Counterbore or countersink diameter.
H2 - Counterbore depth.
Ang - The taper angle per side for the tapered hole type.
End
Sets the desired hole end condition. Select Blind, Until Face, or Thru-All from the drop down list.
Blind - The H1 dimension input field is activated to specify the hole depth.
Until Face - A face will be selected to specify the depth.
Thru-All - The hole will pass completely through the part.
Boundary
If the End condition above is set to Until Face, select the boundary face where the hole should stop.
Tip
The total included tip angle for blind holes. If no value is specified, the bottom of the hole will be flat.
Direction
By default the hole feature(s) will be perpendicular to the Face input above. You can use this option to select a different centerline direction.
File/Bundle
Use these options to load and save hole attribute bundles and to look-up the attributes of an existing hole feature. See Attribute Bundles and Form Commonalities for more information about these options. Also refer to the Hole Standards Library section below.
Save
This saves the form's current attributes to an attribute bundle associated with the active file. In the popup Save Attributes Form, enter a name for a new bundle and pick OK or double-click on an existing bundle in the list to overwrite it. The name will be displayed in the Bundle List . Select it to display the bundle's attributes.
Use these options to specify thread attributes. You can use them to display cosmetic threads in layout views if the Show threads option is checked on the View Attributes Form or on the options forms for the various layout view creation commands.
In order to maintain standard thread attributes, the values for thread Diameter are limited depending on the Type selected. You can cycle through the available values. The values for Pitch or Threads/Unit are set automatically depending on the Diameter. You can change the value if more than one is available. If Type is set to Custom, you are free to enter any desired diameter and the Pitch or Threads/Unit values will adapt accordingly.
As the thread diameter and pitch are selected a suggested value is also made for D1, the pre-drilled or tap hole diameter. The value for D1 may vary depending on the amount of contact with the thread so a valid value is selected, but you may modify this if you choose. All values are in the current part units defined in the Part Settings Form.
Type - Select the standard for the type of thread attributes to apply or select No Thread if you don’t want thread attributes applied to the hole. The thread standards supported include UNC, UNF, M (metric) and Custom. The values for Diameter, Pitch and Threads/Unit (see below) will conform to standard Type selected.
Diameter - Specifies the outer thread diameter. This is also referred to as the "basic major diameter" for standard threaded holes.
Pitch or Threads/Unit - Specifies the thread by either Pitch or Threads/Unit. Select one and enter the value.
Depth - Specifies the depth of the thread into the hole feature.
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Use these options to specify hole tolerance attributes.
Add D1 tolerance - Check this box to use tolerance attributes.
Upper limit (+) - The positive max. tolerance value (e.g., for +0.005, enter 0.005 here).
Lower limit (-) - negative max. tolerance value (e.g., for -0.005, enter 0.005 here)
Callout label - Any text string that you want to appear as the hole callout. This label is supported by the Hole Callout Dimension command at the Drawing Sheet level. You can set the decimal places for hole callout labels using the General tab of the Dimension Attributes Form (select Attributes > Dimension).
Do not machine - Holes flagged with this attribute are ignored in VX CAM. For example, a plate loaded from a catalogue has holes that already exist -- VX CAM will not machine them.
Bundles.VX
VX has predefined hundreds of standard hole attributes into a library called "Bundles.VX" stored in the "driver/resource" folder of your User Directory.
These are standard holes based on the "Machinery's Hand Book" and include thread and tolerance values. These values are stored to the 6th decimal place to meet the standard.
Pick the folder icon on the Hole Feature Options Form and use the File Browser to locate the "Bundles.VX" file (if it's not already selected) and then select a hole from the drop-down list. The options form will populate with the selected hole's attributes.
