Part Modeling > Part Modeling > Engineering Features > Hole > About the Hole Feature User Interface
About the Hole Feature User Interface
The Hole tab consists of commands, tabs, and shortcut menus. Click Model > Hole to open the Hole tab.
Commands
Type
Simple—Displays the simple hole options.
Standard—Displays the standard hole options.
Profile
Simple type is selected:
Flat—Creates straight, cylindrical holes.
Drilled—Creates drill-shaped holes.
Sketched—Uses a sketched profile that you create in Sketcher.
Standard type is selected:
Straight
Tapped—Creates threaded holes.
Drilled—Creates drilled holes that are not threaded.
Clearance—Creates clearance holes.
Tapered—Creates tapered holes.
Countersink—Adds a countersink.
Counterbore—Adds a counterbore.
Size
Simple type is selected:
Flat or Drilled profile are selected:
Diameter—Sets the hole diameter.
Sketched profile is selected:
Open—Opens an existing sketched profile.
Sketch—Opens Sketcher to create a profile.
Standard type is selected:
Thread type—Sets the thread type
Screw size—Sets the screw size.
Depth
Depth options:
Blind—Sets depth from the placement reference to a specified depth value.
Depth box—Sets the depth value.
Symmetric—Sets half the depth value on each side of the placement reference.
Depth box—Sets the depth value.
To Next—Sets the depth to the next surface of a solid.
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This option is not available in these cases:
On the Body Options tab, All is selected
On the Body Options tab, more than one body is in the Selected collector
In Assembly mode
Through All—Sets the depth through all surfaces.
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For holes created at the assembly level, when Through All is selected for the hole depth, Through Thread cannot be selected for the thread depth.
Through Until—Sets the depth to the selected surface.
Reference collector—Displays the surface that sets the hole depth.
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This option is not available in these cases:
On the Body Options tab, All is selected
On the Body Options tab, more than one body is in the Selected collector
In Assembly mode
To Reference—Sets the depth to the selected point, curve, plane, surface, quilt, or body.
Reference collector—Displays the point, curve, plane, surface, quilt, or body that sets the hole depth.
Drilled hole depth measurement method:
Shoulder—Measures depth to the end of the cylinder.
Tip—Measures depth to the tip of the hole.
Options
Lightweight—Sets a lightweight representation of the hole to improve performance.
Tabs
Placement
Type list
Placement type is context sensitive based on the references selected.
Linear—Two linear dimensions. This type is available when you reference a planar, cylindrical, or conical solid surface or a datum plane. You can also create a linear hole by referencing a datum axis or the axis of an existing hole if the axis is normal to the primary placement reference of the new hole.
Radial—A linear and an angular dimension. This type is available when you reference a planar, cylindrical, or conical solid surface or a datum plane.
Diameter—Rotate the hole around a diameter reference. This placement type uses an axis in addition to linear and angular dimensions. This type is available when you reference a planar solid surface or a datum plane.
Coaxial—A linear and axial reference. This type is available when you reference a surface, datum plane, or axis.
On Point—A datum point located on a surface, offset from a surface, or projected onto a surface. This placement type is available when you reference a datum point.
Sketched—Places holes on sketched datum points, and endpoints and midpoints of sketched straight lines.
—Reverses the placement direction to the other side of the placement reference.
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is available only for simple and standard holes that use the Blind, To Next, or Through All depth options.
Placement collector—Collects the primary placement reference.
Sketch collector—Collects the primary placement sketch when the placement type is Sketched.
Define—Opens the Sketch tab for you to sketch the datum points and straight lines to use as references for holes.
Edit—Opens the Sketch tab for editing the internal sketch.
Unlink—Breaks the association with the selected sketch, and copies the sketch as an internal sketch.
Place holes on:
Points—Places holes on sketched datum points.
Endpoints—Places holes on endpoints of sketched straight lines.
Midpoints—Places holes on midpoints of sketched straight lines.
Offset references table—Displays the offset placement reference information. Available when the placement type is Linear, Radial, or Diameter.
The table contains the following items:
Offset references collector
Reference type:
Offset—Offsets the hole from the secondary reference. This option is displayed if you select the Linear primary placement reference and a secondary placement reference.
Align—Aligns the hole center to the secondary reference. This option is displayed if you select the Linear primary placement reference.
Angle—Uses the secondary reference to determine the hole angle. This option is displayed if you select the Radial or Diameter primary placement reference type and a secondary reference (not including an axis).
Radius—Uses the secondary reference to determine the hole radius. This option is displayed if you select the Radial primary placement reference and select an axis as the secondary reference.
Diameter—Uses the secondary reference to determine the hole diameter. This option is displayed if you select the Diameter primary reference and an axis as a secondary reference.
Reference value box—Controls the secondary placement reference. Type new value or select a recently-used value from the list.
Hole orientation
Hole orientation collector—Displays a planar, axial, or linear reference to optionally define the orientation of the hole.
Hole orientation options—Sets the hole orientation in relation to the orientation reference.
—Sets the hole parallel to the orientation reference.
—Sets the hole perpendicular to the orientation reference. When the orientation reference is planar, the hole can only be perpendicular to the hole orientation reference.
Dimension orientation reference collector—Available for Linear holes when the axis of a hole or a datum axis that is normal to the primary reference is selected as the secondary reference.
Shape
The Shape tab defines hole geometry and illustrates it. Some of the options are context sensitive according to the hole type.
Simple (straight) holes:
Flat rectangle profile:
Side 2 depth options box—Sets the depth options for Side 2. Displays the same depth options as those listed above.
Side 1 depth options box—Sets the depth option for Side 1. Displays the same depth options as those listed above.
—Sets the hole diameter.
Drilled hole profile
Side 1 depth options box—Sets the depth option for Side 1. Displays the same depth options as those listed above.
—Sets the hole diameter.
When the Blind depth option is selected:
Drill point angle box—Controls the angle of the drill point for Blind standard hole profiles.
Drilled hole depth measurement method:
Shoulder—Measures depth to the end of the cylinder.
Tip—Measures depth to the tip of the hole.
When Countersink is selected:
Countersink angle box—Sets a value for the countersink angle.
Countersink diameter box—Sets a value for the countersink diameter.
When Counterbore is selected:
Counterbore depth box—Sets a value for the counterbore depth.
Counterbore diameter box—Sets a value for the counterbore diameter.
When Through All is selected:
Exit Countersink check box—Adds countersink drilling at the bottom of the hole and if the hole exit surface is parallel to the primary placement reference surface. This check box is not available in Assembly mode, for holes using the Sketched placement type, or when cut geometry from All bodies is selected.
Sketched (straight) profile—Displays only the sketch geometry in an embedded window.
Standard holes
Straight profile
Tapped
Thread depth options:
Through Thread—Threads the entire depth of the hole.
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For holes created at the assembly level, when Through Thread is selected for the thread depth, Through All cannot be selected for the hole depth.
Blind—Threads to a specified depth value.
To Reference—Threads to the selected surface, quilt, body, plane, edge, curve, axis, point, or vertex.
Include thread surface check box—Creates a thread surface to represent the internal threads of the standard hole.
When Blind is selected:
Drill point angle box—Controls the angle of the drill point for Blind standard profile holes.
Clearance (non tapped) hole:
Fit box—Defines the hole clearance diameter:
Close Fit—Creates a fit intended for the accurate location of parts which must assemble without perceptible play.
Medium Fit—Creates a fit suitable for ordinary steel parts or for shrink fits on light sections. The medium fit is the tightest fit that can be used with high-grade cast iron external members.
Free Fit—Creates a fit intended for use where accuracy is not essential, where large temperature variations are likely to be encountered, or both.
—Diameter box is available when you select certain screw sizes.
Tapered
Straight drill depth options:
Blind—Drills from a placement reference to a specified depth value.
To Next—Drills to the next surface.
Through All—Drills through all surfaces.
Through Until—Drills to intersect with the selected surface.
To Reference—Drills to the selected surface, quilt, body, plane, curve, or point.
None—Does not add a straight drill.
Tapered tip check box—Adds a slanted surface at the bottom of the tapered drill.
Thread length—Length of the thread measured from the hole placement plane, or for holes with a counterbore, from the counterbore plane. The thread length can be greater than the drill depth in tapered holes.
Drill depth
The Standard hole contains a Countersink:
Countersink angle box—Sets a value for the countersink angle.
Countersink diameter box—Sets a value for the countersink diameter.
The Standard hole contains a Counterbore:
Counterbore depth box—Sets a value for the counterbore depth.
Counterbore diameter box—Sets a value for the counterbore diameter.
When Through All is selected:
Exit Countersink check box—Adds countersink drilling at the bottom of the hole and if the hole exit surface is parallel to the primary placement reference surface. This check box is not available in Assembly mode, for holes using the Sketched placement type, or when cut geometry from All bodies is selected.
Top Clearance check box—Ensures that the entire top of the hole intersects the outside of the solid geometry. The top of the hole feature extends outward using a cylinder with a diameter equal to the top of the hole, including a counterbore or countersink, and removes material so that the top of the hole is not fully or partially buried.
Intersect
This tab is available only in Assembly mode. Refer to the Assembly documentation for more information.
Note
Displays thread notes for Standard holes. Available only if Standard is selected.
Add a note check box—Creates a note.
Reset—Restores the default note created during initial feature creation.
Thread notes are also displayed in the Model Tree and in the graphics window after you create the hole. To view the notes, in the Model Tree, click > Tree Filters. The Model Tree Items dialog box opens. Under Display, select the Annotations check box and click OK.
Body Options
Not available for creating assembly-level features.
Cut geometry from body
All—Cuts geometry from all the bodies that the feature passes through.
Selected—Cuts geometry from the selected bodies.
Body collector—Selects the body from which geometry is removed.
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The body that is selected in the collector on the Body Options tab cannot be used as a depth reference.
Properties
Name box—Sets a name for a hole feature.
—Displays feature information in a browser.
Parameters table—Displays a customized hole chart data. To modify parameter names and values, modify the hole chart file. This table is available only for Standard holes. The Parameters table contains the following items:
Name—Contains the name of each customized column in the hole chart file.
Value—Contains the value associated with the corresponding Name column.
Shortcut Menus
Right-click the graphics window any place except over a handle to access shortcut menu commands:
Lightweight—Sets a lightweight representation of the hole to improve performance.
Flip—Reverses the placement direction of the hole. Flip is available only for simple and standard holes that use the Blind, To Next, or Through All depth option.
Placement type options for holes:
Linear—Two linear dimensions. This type is available when you reference a planar, cylindrical, or conical solid surface or a datum plane. You can also create a linear hole by referencing a datum axis or the axis of an existing hole if the axis is normal to the primary placement reference of the new hole.
Radial—A linear and an angular dimension. This type is available when you reference a planar, cylindrical, or conical solid surface or a datum plane.
Diameter—Rotate the hole around a diameter reference. This placement type uses an axis in addition to linear and angular dimensions. This type is available when you reference a planar solid surface or a datum plane.
Coaxial—A linear and axial reference. This type is available when you reference a surface, datum plane, or axis.
On Point—A datum point located on or offset from a surface. This placement type is available when you reference a datum point.
Sketched—Sketched datum points, and endpoints and midpoints of sketched straight lines in an external or internal sketch.
Hole orientation options—Defines whether the hole is parallel to or perpendicular to the orientation reference.
Parallel
Perpendicular
Top Clearance—Ensures that the entire top of the hole intersects the outside of the solid geometry. The top of the hole feature extends outward using a cylinder with a diameter equal to the top of the hole, including a counterbore or countersink, and removes material so that the top of the hole is not fully or partially buried.
Define Internal Sketch—Opens the Sketch tab for you to sketch the datum points and straight lines to use as references for holes.
Edit Internal Sketch—Opens the Sketch tab for editing the internal sketch.
Placement Reference Collector—Activates the Placement reference collector.
Sketch Collector—Activates the Sketch reference collector to collect the primary placement sketch when the placement type is Sketched
Offset References Collector—Activates the Offset References collector.
Hole Orientation Reference Collector—Activates the Hole orientation collector.
Dimension Orientation Reference Collector—Activates the Dimension orientation reference collector. This option is available only if you select Linear as the placement type and an axis of a hole or a datum axis that is normal to the primary reference as the secondary reference.
Clear—Clears the active collector.
Straight Depth—Selects the straight drill depth option for a tapered hole. Options are Blind, To Next, Through All, Through Until, To Reference, or None.
Depth1 Reference Collector—Activates the first direction (side 1) Depth Reference collector. This command is available only for Simple holes that use the Through Until or To Reference depth option.
Depth2 Reference Collector—Activates the second direction (side 2) Depth Reference collector. This command is available only for 2-sided Simple holes that use the Through Until or To Reference depth option from the Side 2 depth options box.
Depth Reference Collector—Activates the Depth Reference collector. This command is available only for Standard holes that use the Through Until or To Reference depth option.
Intersecting Components Collector—Activates the Intersecting Component collector. This command is available only in Assembly mode and Automatic Update is cleared.
Select bodies—Activates the body collector so you can select bodies.
All—Removes geometry from all the bodies that the feature passes through.
Selected—Removes geometry from the selected bodies.
Points—Places holes on sketched datum points.
Endpoints—Places holes on endpoints of sketched straight lines.
Midpoints—Places holes on midpoints of sketched straight lines.
Show Section Dimensions—Shows the internal section dimensions.
Hide Section Dimensions—Hides the internal section dimensions.
Right-click a depth handle to access depth options. These commands are not available for Sketched holes.
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For 1-sided Simple holes, a shortcut menu command drills the hole in the first direction (Side 1). For 2-sided Simple holes, you must place your pointer over the Side 2 depth handle, right-click and use a shortcut menu command to drill the hole in the second direction (Side 2).
Right-click a secondary placement reference handle to access the placement options.
Right-click a collector that contains a reference to access the following shortcut menu commands:
Remove—Removes the selected reference or the reference indicator from the active collector.
Remove All—Removes all references from the active collector.
Information—Opens the INFORMATION WINDOW to display detailed reference information pertaining to the selected reference in the collector.