SpaceClaim Online Help

Inserting a standard hole

The Standard Hole tool creates industry standard drilled and tapped holes. Select one of the available standards (ISOInternational Organization for Standardization standards for architectural and engineering drawing, including guidelines for dimensioning and tolerancing. You can customize the style of your annotations to conform to ISO standards. See ASME, JIS., UNC, etc.) and then choose from available sizes and specify other hole characteristics (Blind, Tapped, Countersink, Counterbore, Drill point details).

The current hole profile is displayed in the Preview group. It dynamically updates as you define the hole. There is also a gallery of common hole profiles to choose from.

Hovering over the Preview shows the hole's definition, as it would appear in a Hole Table.

While choosing a placement location, a preview of the hole opening, including countersink and/or counterbore, is attached to the cursor. This allows you to view the footprint of the hole as you locate it.

Standard hole creation overview

1. Click  Standard Hole in theManufacturing group of the Insert tab.

   The Hole Toolbar opens. GroupsSets of objects that appear in the Groups tab. You create a group from any set of selected objects. Information such as Selection, Alt+selection, move anchoring, axis, and ruler dimension is all stored with the group. in the toolbar contain the options and inputs for hole definition.

2. Set options and enter values to define the hole.

   • Choose a Series, Size, and Fit
     • The Series you choose determines the available sizes and Fit options
   • Choose treatments:
     • Blind depth
     • Tapped thread depth
       • When Tapped is checked, diameter displays tap drill size
       • When Tapped is checked, Fit is disabled

       • May be determined by Series and Size. If so, you can still enter a different value. The value you enter will be displayed in bold font to indicate it is non-standard

       • Default thread depth is twice the basic hole diameter

       • NoteAnnotation placed on a design, drawing sheet, or 3D markup. Notes contain text or symbols that you insert and can be connected to geometry by a note leader. that only the most common Standard Hole sizes have cosmetic display
       • Cosmetic threads appear in the Structure treeDisplay in the Structure panel that shows you each of the objects in your design. You can expand or collapse the nodes of the tree to view the objects. You can rename objects, create, modify, replace, and delete objects, as well as work with components. and can be toggled on/off
     • Cosmetic thread depth
       • Cosmetic threads are only available for the UNC series
       • Cosmetic threads show a thread helix without actual thread geometry

         

   • Choose a Style: Countersink, Counterbore, or both

     • Countersink   Counterbore          Both

                  

     • Diameter and Angle

       • Determine countersink depth

       • Some Series specify both dimensions, some specify one, and others specify none

       • If they are specified, you can still enter a different value but it will be displayed in bold font to indicate it is non-standard

     • Diameter and Depth

       • Some Series specify both dimensions, some specify one, and others specify none
       • If they are specified, you can still enter a different value but it will be displayed in bold font to indicate it is non-standard
   • For Blind holes, you can specify a Drill point
     • Enter a Drill point angle
     • Choose Drill point depth measurement type
       • Depth to Shoulder  
       • Depth to Tip  

   Preview shows the hole profile based on current selections and values. Shown below is a Blind, Tapped, Countersunk, and Counterbored hole with Drill point details.

    

   

    

   As you work with different inputs, Preview gives visual feedback. Below are examples of what you would see when entering values for Diameter, Hole Depth, Countersink Angle, and Drill point Angle.

    

                    

    

   Preview also has a gallery of profiles to choose from. Click on the Preview image to open the gallery.

   The gallery is a graphical way to define the hole. Selecting a hole from the gallery automatically fills in the details in the ribbon.

    

   

    

3. Choose a tool guide for hole placement.

   •  SnapConstrain to objects, angular and linear increments, or grid points while you are sketching or editing solids. You can customize the snapping behavior in File>Options. Pressing Shift while dragging snaps the tool based on your snap settings. You can use the Snap to grid tool to constrain or lock all drawing to grid points only. to GridSee Sketch grid

     Select a face on which to display the sketch grid. As you move the cursor, the hole center will snap to the grid points.

   •  Free Placement

     Pick anywhere on any face to locate the hole center.

      

4. Place the hole by clicking in the desired location.
   • You can continue to place this type of hole at more locations, or you can change values and options to place different types of holes.
   • All holes show in preview until you decide to complete them.
   • You can place holes using a plane that is some distance away from the face. This is useful if the hole needs to be on a curved face.

     

5. While the holes are previewed, you can:
   • Ctrl+click a hole preview to remove it from the set of holes to be created.
   •  Press the Escape key to clear all previews without exiting the tool.

6. Complete the hole(s) by clicking  Complete. All previewed holes will be completed. You can also double-click when you place a hole to complete it.

7. Continue to make more holes or leave the Hole toolbar.

8. Click in the Close group to close the toolbar.

Hole Series

Hole Size and Fit options are determined by which Series you choose.

The examples below show the difference between ISOInternational Organization for Standardization standards for architectural and engineering drawing, including guidelines for dimensioning and tolerancing. You can customize the style of your annotations to conform to ISO standards. See ASME, JIS. and UNC. Notice the change in Size nomenclature and Fit options. ISOInternational Organization for Standardization standards for architectural and engineering drawing, including guidelines for dimensioning and tolerancing. You can customize the style of your annotations to conform to ISO standards. See ASME, JIS. has Fit options of Nominal, Close, Medium, and Free.

Fit is disabled in UNC. 

• Within each Series, the Size you choose determines the hole diameter
• You can enter a different diameter and it will be shown in Bold to indicate that it is non-standard 

As of SpaceClaim 2014 SP1, the NPS series is replaced by NPSM. Standard Holes created using NPS in existing models will not be recognized.

Customizing Hole Series

• Series and Size determine the values in the rest of the Hole ribbon inputs.
• All of the information to update the inputs is contained in XML files located in the <SpaceClaim loadpoint>\Libraries\Holes directory.
• Each series has a corresponding XML file. 

The image below shows the ISOInternational Organization for Standardization standards for architectural and engineering drawing, including guidelines for dimensioning and tolerancing. You can customize the style of your annotations to conform to ISO standards. See ASME, JIS. M18 x 2.5 ribbon.

The XML for this ISOInternational Organization for Standardization standards for architectural and engineering drawing, including guidelines for dimensioning and tolerancing. You can customize the style of your annotations to conform to ISO standards. See ASME, JIS. hole size is in the ISOInternational Organization for Standardization standards for architectural and engineering drawing, including guidelines for dimensioning and tolerancing. You can customize the style of your annotations to conform to ISO standards. See ASME, JIS..xml file. The relevant XML is shown below.

Notice the correspondance between the XML tags and the ribbon inputs.

All dimensions are in millimeters and angles are in degrees.

The image below shows the result of switching to the UNC Series and the 3/4 - 10 Size.

The XML for this UNC hole size is in the UNC.xml file. The relevant XML is shown below.

• Notice the correspondance between the XML tags and the ribbon inputs.
• All dimensions are in inches and angles are in degrees.

The image below shows the values in the XML file show up in a Hole Table created in a drawing.

You can edit any of the series XML files to customize the series.

• NoteAnnotation placed on a design, drawing sheet, or 3D markup. Notes contain text or symbols that you insert and can be connected to geometry by a note leader. that edited files will be overwritten the next time you upgrade to a newer version of SpaceClaim
• Any changes made to the XML files, do not go into effect until you restart SpaceClaim

 It is recommended that you customize the series by adding files to the directory.

• New files add items to the Series drop-down menu
• Deleting files or moving them out of the directory removes items from the Series drop-down menu

The image below shows a "DCZ" series added.

The DCZ series is based on UNC by copying UNC.xml to DCZ.xml and editing the sizes. 

• NoteAnnotation placed on a design, drawing sheet, or 3D markup. Notes contain text or symbols that you insert and can be connected to geometry by a note leader. the new TapDrill value reflected in the Diameter input and the new Countersink and Counterbore values.

Drill Chart

Drill chart is a Series based only on Diameter values. It refers to a set of XML files that contain hole definition tables. Edit the files to customize the Standard Hole tool.

In the <SpaceClaim loadpoint>\Libraries\Holes\Drills directory, you will find the following files:

• Fraction.xml
• Letter.xml
• Metric.xml
• Number.xml

File names refer to how the hole name is specified. Below is an example from Letter.xml.

<Name>A</Name>

<Diameter>0.234</Diameter>

<ImperialDisplay>0.234</ImperialDisplay>

<MetricDisplay>5.94</MetricDisplay>

Modify the files according to this format to define custom holes.

To create a hole using Drill chart

1. Select Drill chart as the Series.
2. Enter a Diameter.
   • Enter a letter, decimal value, fraction (1/64, 3/32, etc.), or number (#1, #2, etc.)
   • Units are assumed but can be overridden. For example, if Units are metric, 5.94 is assumed to be 5.94mm. Override the default by entering 0.234".
3. Diameter as entered is matched to the corresponding hole in the appropriate chart. Hover over the Preview to see the callout information.
4. Place the hole on a face.
5. Click Complete, or double-click.

Hole Selection

SpaceClaim recognizes Standard Holes. Hovering over a hole face will pre-highlight the hole object.

Select individual hole faces using query select.

Deleting any Standard Hole face, or the face it was created on, breaks the Standard Hole association. Individual faces are still selectable, but are not recognized as a Standard Hole. 

To edit a Hole

1. Select the hole to modify.

   You can also CTRL select, or box-select, several holes that share any of the same parameters.

2. Open the Standard Hole Edit tab. You can also double-click a Standard Hole to open the Edit tab.

   The Edit tab is not available for multiple holes that share no parameters.

3. Edit the Hole definition.

4. You can continue to select and Edit more holes.

5. To close the Edit tab:

   • Select a non-hole object

   • Click white space in the Design windowArea in the user interface that displays your model or assembly. Also known as Workspace.

   • Enter selection for another tool

With a Standard Hole selected, you can use the Reverse Hole option in the context menu to flip the hole to the opposite side of the part.