I just heard my first Christmas carol this year. It was “These are a few of my favourite things”, sung by Julie Andrews. It got me thinking two things. First; it’s still too early for Christmas and second; this would be a good idea for our blog. When I teach advanced classes, I am often amazed how many basic tips and tricks, that I take for granted, are not known by the average user. So here are few of my favourite, yet often overlooked, useful tips and tricks in Solid Edge.
Sketching Tips and Tricks
The A key in the line command
This line command draws a continuous series of lines and arcs that can be perpendicular or tangent to each other. Note that it says lines and arcs. Many users are not aware of the arc capability in the line command.
This command starts in line mode by default. If you want to start by drawing an arc, press the A key on the keyboard, or click the Arc button on the command bar. Once the arc is drawn the command defaults back to line mode.
Snap-to-point shortcut keys
Once you have located an element with the cursor, you can use the following shortcut keys to snap to keypoints and intersection points.
• Midpoint - press M.
• Intersection point - press I.
• Center point - press C.
• Endpoint - press E.
Tip: To help you remember what the shortcut keys are, note that the letters can be arranged to spell the word mice.
Ctrl key to focus scroll wheel control
However, if you move the cursor off the dimension field, the focus of the scroll wheel changes to zoom in and out. To avoid this hold down the Ctrl key and the focus of the scroll wheel remains on the dimension field.
Note: You can have the scroll wheel set to always focus on the dimension field, by toggling on the options in Solid Edge Options>General tab.
Keyboard options for the Smart Dimension Command
Before you click to place the smart dimension, you can use the following keys to affect the dimension that is created. The options that are available depend upon what, and how many, elements you select. Refer to the specific prompts displayed on PromptBar as you select elements.
Part Modeling Tips and Tricks
Replace Face command
This command replaces selected faces on a part. The replacement face can be a construction surface, a reference plane, or another face on the part. When replacing more than one face, the faces being replaced cannot touch each other.
When you replace a face using a construction surface, the construction surface is hidden automatically when you finish the feature.
If edges on the face you are replacing have rounds applied, the rounds are reapplied after you complete the replace face operation.
Steps to replace a face
1. Choose Surfacing tab→Surfaces group→Replace Face .
2. Click the face you want to replace and then click the Accept (check mark) button on the command bar.
3. Click the surface you want to replace the face with.
4. Finish the feature.
With this command you can remove the tool body volume from selected target bodies. You can select multiple target bodies and multiple tool bodies. The tool body can be a design body or construction body.
You can also use a reference plane or a surface as the tool. These tools have no volume. You choose a direction to subtract volume from the target body.
You can preset the type of output body to create if the resulting body is a non-manifold by using one of the following options on the Boolean Options dialog box.
• Create multiple bodies
• Fail (no output)
Lock and Unlock PMI dimension form the PathFinder
By clicking on the lock icon in the Pathfinder, users can lock or unlock PMI dimensions in the synchronous paradigm.
Assembly Tips and Tricks
The FlashFit option reduces the steps required to position parts using mate, planar align, and axial align relationships when compared to the traditional workflow. Because many parts are positioned using these relationships, FlashFit is appropriate in most situations.
When you position a part using FlashFit, you first select a face or edge on the placement part. You then select a face or edge you want on the target part and let the inference logic built into Solid Edge determine the most likely relationship, based on the target part element.
A Flip button on the command bar allows you to select the alternate solution. You can also use the Tab key to select an alternate solution.
FlashFit also allows more flexibility to use edges, in addition to faces, when positioning a part using mate, axial align, and planar align relationships.
Note: The Flip option or the Tab key selects an alternate solution if desired.
Capture Fit command
Use the Capture Fit command to capture the assembly relationships and faces used to position a part or subassembly already placed in the assembly. You can then place the part or subassembly again later using fewer steps. This command is ideal for hardware and commonly used parts. When you drop the part into the assembly document, the faces of the placement part highlight and you are prompted to select the corresponding faces on the target part. With capture fit parts, you can fully place a part in 3 clicks.
You can use the Capture Fit dialog box to specify which relationships you want to capture.
Steps to capture the assembly relationships for a part
1. In the assembly window, select a part for which you want to capture relationships. Note: the assembly relationships must already exist on this part.
3. In the Capture Fit dialog box, use the Add and Remove buttons to specify which relationships you want to capture, and then click OK.
• You can also select the part you want to use in PathFinder.
• When you use the Capture Fit command, the relationships and faces used to position the part or subassembly the first time are stored so you can place the part using fewer steps later.
• If you used the Insert option to position a part, the Capture Fit command will capture a mate and an axial align relationship, since these are the relationships that the Insert option actually places.
• The Capture Fit command cannot capture angular, cam or center-plane relationships.
Drafting Tips and Tricks
Creating drawing views from a model dragged onto a sheet
Another way to create drawing views is to drag a model onto a drawing sheet. When you do this, the View Wizard command runs automatically to create the drawing views. This produces a
standard drawing view based on the type of model. The view orientation of the first view placed is shown in the following table.
Example: If you drag a part or sheet metal model onto the sheet, a standard set of views is generated and placed.
Example: The first view placed in an assembly model is an isometric view. After placing the first view, you can create additional views from the primary view by moving the cursor and clicking to place each one.
Updating Views tips
• To update a single drawing view, select the drawing view and click the Update View command on the shortcut menu.
• Force Drawing Views to Update--If you hold Ctrl+Shift when you click Update View, Solid Edge performs a full update, just as it would on initial view creation. That is, it rereads all of the model data to regenerate the view, rather than only the model data thought to have changed.
Now obviously there are many more tips and tricks available, but these are some of my favourite ones, which I feel should be basic knowledge. More information can be found on these commands in the Solid Edge Help docs. If you are a Designfusion customer, you can always get more detail by contacting our support desk at 1-877-215-1883 or email us at [email protected]