Dimensioning in Solid Edge ST
Introduction
This tutorial illustrates the typical workflow for creating and placing drawing views, and dimensioning and annotating the views of the machined part shown in the illustration above. This workflow is applicable to both synchronous models and traditional models in Solid Edge ST.
You will learn to do the following:
- Place a principal Front view plus three other standard views (Top, Side, and Isometric) using the Drawing View Creation Wizard.
- Add a detail view using the Detail View command.
- Use a cutting plane to create a section view, and then place the view on the drawing using the Section View command.
- Adjust the position of views on the drawing.
- Add drawing view labels.
- Change and show drawing view scale.
- Open the model from the drawing to make a change, and then update the drawing views.
- Retrieve dimensions from the model.
- Add new dimensions to the drawing views, such as:
- Distance between
- Chamfer dimension
- Modify the format of dimensions:
- Text location and size
- Terminator placement
- Dimension line location
- Add a variety of annotations:
- Smart Hole callout
- Center line
- Datum frame
- Feature control frame
Select Units and Type of Operation
The first tasks are to change the units to millimeters, and type of operation available. The standard units used with the default installation of Solid Edge are ISO (millimeters), but some installations may have used ANSI (inches) instead. If so, you need to change to millimeters for this tutorial. Once you have started execution of the Solid Edge program in Windows, you will see a screen similar to the one shown below. If the options in Createare the ones shown, you will need to make two changes before you can start the tutorial. If the option ISO Draftis available, select it and go the next part of this tutorial labeled Specify the dimensions of the drawing sheet.
Otherwise, select the icon in the upper left corner of the screen, which will bring up the following window.
Select the Solid Edge Options at the bottom of the screen which will bring up the following window.
Within this window, select User Profile, then use the down arrow next to User type and select Traditional and Synchronous. SelectOK. This will change the start up screen to be the following, which will allow you to select “Traditional” part construction.
The next step is to change the units to ISO. Select the icon in the upper left corner and then select New as shown.
This will bring up the following window.
Within this window select More and then iso draft.dftand then OK. Now you can start the construction of the model.
Specify the dimensions of the drawing sheet
The first step in beginning a new drawing is to set up the drawing sheet.
/ Click the Application button to open the Application menu./ From the Application menu, choose Sheet Setup.
On the Sheet Setup dialog box, on the Size tab, set the Sheet Size option to A3 Wide (420 mm x 297 mm).
Click the Background tab, and set the Background Sheet option to A3-Sheet.
On the Sheet Setup dialog box, click OK.
Fit the drawing sheet to the window
On the status bar at the bottom of the application window, click Fitto fit the drawing sheet to the window size.
The Fit command is conveniently located on the status bar at bottom-right of the application window, along with other view manipulation commands. You can use these commands at any time to adjust the view. For example, you can begin drawing a cutting plane line, and then realize you need to zoom in to draw it.
To exit a view manipulation command and return to a drawing command in progress, press Esc.
Set the projection angle
Mechanical drafting standards use either a first-angle projection or a third-angle projection for creating multi-view projections of a part on a drawing sheet. The first-angle method is predominantly used by engineers and designers who follow ISO and DIN (metric) standards. The third-angle method is predominantly used by engineers and designers who follow ANSI (English) standards.
Since we are using the ISO standard in this tutorial, Solid Edge is automatically in first angle projection. This tutorial illustrates both first-angle and third-angle projection. However, change to third-angle projection now. To do this select icon in the top left corner of the screen and then the Solid Edge Options.
On the Drawing Standard page, under Projection Angle, select Third for third-angle projection, and then OK.
Choose a part model to place on the drawing sheet
/ On the Home tab>Drawing Views group select the View Wizard command.On the Select Model dialog box, do the following:
- Set the Look In location to the Solid Edge ST Training folder
- Set the Files Of Type option to Part Document (*.par)
- Select the file named DraftTut1MP-DV.par, and then click the Open button.
The default location of the Solid Edge Training folder is:
C:\PROGRAMFILES\SOLIDEDGE ST\TRAINING
However, your system administrator may have chosen a different location.
Ensure that the part view options on the first page of the Drawing View Creation Wizard match the following.
On the Drawing View Creation Wizard, click the Next button.
Specify the orientation of the principal view of the part
On the Drawing View Orientation page of the Drawing View Creation Wizard, under Named Views, select front and then click the Next button to continue.Specify additional views of the part
If you are using third-angle projection, on the Drawing View Layout page of the Drawing View Creation Wizard, select the views shown in the illustration below, and then click Finish.
If you are using first-angle projection, select the views shown below, then click Finish.
Notice that the rectangle attached to the cursor changes size. It now represents the size of the four views you have specified.
Do not click the drawing sheet yet.
Place the views on the drawing sheet
Move the cursor to position the views on the drawing sheet as shown in the illustration below, and click to place them.
Observe the drawing Views
For a third-angle projection, your drawing view arrangement should be similar to this.
Save the file
Select the Save As option using the icon in the top-left corner of the screen and save the part as Tutorial.dft.Change the scale properties of a view
You can change the display size of a view to make it smaller or larger, so there is more room for dimensions and annotations.
Click on the isometric drawing view.
In the Select command bar, click the Scale list, and select 1:2.
The isometric view updates automatically on the drawing sheet.
Click the Show Scale button.
Create and display a caption for the isometric view, by:
- In the Caption box on the command bar, type Scale.
- Press Enter.
- Click the Show Caption button.
The resulting isometric view is:
Reposition a view on the drawing sheet
You can adjust the position of a view by dragging it.
/ Verify that the Select command on the Home tab>Select group is active.- Position the cursor over the view you want to move, so that it highlights and the cursor changes to a circle.
- Hold the left mouse button while you drag the view.
- Release the mouse button.
Use the technique described above to adjust the spacing of the views on the drawing. When you drag the Front or Top view, the other view moves with it to maintain proper drawing view alignment.
For the third-angle projection, position the views as shown.
When you move one of the primary views, such as Front, Right, or Top, drawing view alignment lines are displayed to help you maintain proper view alignment on the drawing sheet. This is also true for section and auxiliary views.
You can temporarily disable drawing view alignment by right-clicking the view, and then clearing the Maintain Alignment setting on the shortcut menu. This enables you to reposition the view independently on the drawing sheet. The section view remains completely associative to the original part.
Create a detail view
It requires just three clicks to create a detail envelope and place a detail view using default properties for envelope shape, caption, and scale.
/ On the Home tab>Drawing group, click the Detail button.In the Side view, click the center of the area where you want to create the detail. This is the center of the circular detail envelope.
For this tutorial, click the center of the notch. (1)
Move the cursor to the side, and then click to specify the diameter of the circular detail envelope. (2)
The detail view envelop now is attached to the cursor. Move the cursor to position the detail view where you want it on the drawing, and then click. (3)
Before you create the detail view, you can change the default settings on the Detail View command bar.
- The default detail view scale is two times the scale of the view it was derived from. You can change the Scale before you place it, or you can change the scale later.
- The default detail envelope shape is a circle, but you can draw a user-defined envelope shape using the Define Profile option.
- The default detail view updates with changes to the view it is derived from. You can select the Independent Detail View option to create a detail view that is independent of the source view.
Show the scale of the detail view
The detail view caption is displayer automatically on the drawing, but the view scale is not.
/ Verify that the Select command on the Home tab>Select group is active.On the drawing sheet, click the detail view. On the Select command bar, click the Show Scale button.
The drawing view updates immediately to display the drawing scale.
After you place the detail view, you can change its properties by clicking the view and then using the options on the Select command bar.
- You can edit the default caption and control its visibility.
- You can control the visibility of the source view annotation.
- You can change the default settings for detail view creation by editing its properties.
- You can adjust the area shown in the detail view by selecting the detail envelope on the source view and moving it.
- You can change the shape and size of the detail view by double-clicking the envelope on the source view, and then using the 2D geometry modification handles to change it. When you are done, you need to click Close Detail Envelope on the ribbon.
Move the detail view
To make room for a section view, use the technique you learned previously to adjust the position of the Detail A view and its source, the Side view.
/ Verify that the Select command on the Home tab>Select group is active.If you are using third-angle projection, adjust the position and spacing so that the drawing looks like this.
Save the file
/ On the Quick Access toolbar at top-left of the application window, click the Save button to save your work.Draw a cutting plane line for a section view
Creating a section view is a simple, three-step procedure:
- Draw a cutting plane line.
- Specify the section view direction.
- Create the section view using the cutting plane line.
/ On the Home tab>Drawing Views group, click the Cutting Plane command.
On the drawing sheet, click the Top view. The command bar displays the 2D drawing options. The Line command is active.
Zoom in on the view. One way to zoom in is to click the + button on the Zoom slider at bottom-right of the application window, or drag the slider to the right.
Draw the cutting plane line horizontally through the two holes in the part, as shown below.
As you draw, notice that IntelliSketch is active, so you can locate the centers of the holes as you draw the lines.
- Place the cursor on a hole, but do not click. Notice that the circle highlights and that a center mark appears at the center of the circle. Now, move the cursor to the right or left of the view, and then click to start the line.
- Move the cursor to the opposite side, making sure the horizontal indicator is displayed, and then click.
- Right-click to end the line.
/ On the ribbon, click Close Cutting Plane. The cutting plane line options are hidden.
Specify the section view direction
In the Top view of the drawing sheet, move the cursor above and below the cutting plane line, and notice that the section view direction arrows flip as the cursor crosses the cutting plane line.
For third-angle projection, move the cursor so the section view direction arrows point up, and then click.
/ On the status bar at the bottom of the application window, click Fit.Create a section view
You use the cutting plane defined previously to create the section view. You cannot use a cutting plane in more than one view.
/ In the Home tab>Drawing group, select the Section command.Click the cutting plane line you created previously. Click where you want to place the section view. Press Esc to end the command.
A close-up of the section view annotation for third-angle projection looks like this:
If needed, select one or more views to adjust the spacing between them.
Turn off hidden line display in the section view
Click the Select command if it is not already active, and then click the section view.
/ On the Select command bar, click the Properties button. The High Quality View Properties dialog box is displayed. Click the Display tab.Clear the check mark in front of the Hidden Edge Style option.
You may see a dialog box that explains that the change to the display settings you just made affects the default part edge display settings for this drawing view. Click OK.
Click OK to close the dialog box.
/ Click the Fit button.Save the file
/ On the Quick Access toolbar at top-left of the application window, click the Save button to save your work.Edit a hole feature in the model
You can make a design change to the part model by opening the part model from a drawing view.
In this tutorial, we will change the diameter of a hole procedural feature using its edit definition handle. While procedural features and their respective edit definition handles are specific to synchronous models, you can edit a hole in a traditional part model, too.
Place the cursor on the edge of the Front view so that it highlights, and double-click.
The part model document is opened for editing.
/ Click the Fit button to fit the part model to the window.Place the cursor on the hole feature shown below, so that the cylinder highlights, and then click to select it.
Notice where the cursor is in this illustration. Click this edit definition handle, which looks just like text.
The edit definition handle is activated, and a dialog box is displayed near the selected text.
In the Counterbore Diameter box, type 20, and then press Enter.
On the Quick Access toolbar, click Save to save the part model.
On the ribbon, click the X button to close the part document.
The draft document is displayed.
Update the drawing views
The gray shaded outline around each drawing view means the view is out of date. Your change to the model hole diameter caused the drawing views to go out of date.
/ In the Choose tab>Assistants group, select Drawing View Tracker.The Drawing View Tracker lists all of the views on the drawing. This icon indicates that a view is out of date: As you move your cursor down the list, the view highlights on the drawing sheet.