15 Solid Edge tips and tricks from beginner to advanced

1. Find and customize keyboard shortcuts

You can see all of the hotkeys available in Solid Edge by going to the customize menu, accessed from the drop-down arrows on the right end of the quick access toolbar. Click the keyboard tab and select “All Keyboard Assignments” from the “Choose commands from” list. This gives you a single list of all the default and custom keyboard hotkeys assigned in Solid Edge.

To create new hotkeys, change “Choose commands from” to “All Tabs.” Browse to the command you want to create a hotkey for and enter a modifier (any combination of Ctrl, Shift and Alt) and a keyboard key (primary character, symbol, number or function).

The only single-stroke (no modifier) hotkeys you can create are function keys (F1, F2, etc.), although there are some already pre-set.

2. Using Alt shortcut keys in Solid Edge

Alt shortcuts are also available in Solid Edge. These are generally intended as accessibility aids but can be used by anyone for a faster workflow. Press and release Alt on the keyboard and then press and release the main key (or key combination, successively) that appears on the icon you want to access.

3. Single stroke hotkeys for Solid Edge sketches

There are several single stroke hotkeys in Solid Edge to make sketching smoother. Here are the ones you should memorize:

• L for a line
• A for an arc
• S for a line from midpoint or symmetric line
• F3 to lock the sketch plane

A helpful mnemonic for Solid Edge’s IntelliSketch features is MICE:

• M for midpoint
• I for intersection
• C for center point
• E for endpoint

4. Easily create dimensions with Smart Dimension

Solid Edge’s Smart Dimension tool, together with the options in the command bar, can create just about any kind of dimension that you might need. For example, imagine you have two circles of different diameters that are not lined up horizontally or vertically. Here are some dimensioning scenarios:

Just clicking on the two circles gives you horizontal or vertical center to center distances:

Using the tangent option in the command bar can dimension to left or right tangents. It will pick the one closest to where you select:

While you’re placing a dimension, if you press and hold the Shift key, the dimension will be aligned to the shortest distance between the two selections:

5. Use an axis to align dimensions

You can also align dimensions on the axis of your choice with the dimension axis tool.

To establish the dimension axis, click the dimension axis tool in the dimension area of the home tab while sketching, and then click on a line that is parallel to the axis. To make dimensions parallel to that axis, start smart dimension and in the command bar change “Orientation” to “Use Dimension Axis.”

You can also combine the dimension axis with tangent settings:

6. Place dimensions as you sketch

IntelliSketch’s auto-dimension settings allow you to place dimensions as you sketch in Solid Edge. You can automatically create dimensions for new geometry when it’s drawn, including the lengths of lines, radii of arcs and the diameters of circles. You can also set Solid Edge to only add dimensions when you key in a value in the input box during sketching. 

An arc can be described with at least three parameters: radius, included angle and arc length. When you use the smart dimension tool to click on an arc, the first parameter that Solid Edge wants to place is the radius of the arc. If you want the included angle of the arc, just press the A key, and if you want the arc length, press the A key again.  

Solid Edge has some interchangeable names for things. Sketches and profiles are the same things, under different circumstances. A protrusion is a feature that adds material, and an extrusion pushes a sketch along a straight line. A protrusion can also be a revolve.

Solid Edge by default wants you to make features by starting the extrude, picking a sketch plane, and then creating a sketch. This way, all three are linked—the feature, the plane and the sketch. If you delete the feature, the sketch and the plane are also deleted. 

But if you create the sketch, and then create the plane and then create the feature, the sketch and plane are independent of the feature. 

Further, if you create the plane, then create the sketch, then create the feature, all three are independent. If you delete the plane, the sketch just gets a warning, and you can select a new plane for the sketch. If you delete the sketch, the feature gets a warning and you can select a new sketch. 

If you do things the way Solid Edge expects you to do things, the workflow for creating everything is faster, but your editing options are limited.

If you are getting into model based design, you’ll want to start working with model views. Model views are essentially 3D named views saved with sections, PMI and annotations. These can be used to make 3D PDFs. Views can be shown in different render states. Views are saved in the PathFinder with the PMI dimensions, and annotations can also be selected and shown or hidden from the PathFinder.

When you are working toward a goal, you often have to achieve multiple steps in order to get there. Let’s say for example that you have an irregular container, and you want to find the volume. The first step would be to start by making the container shape, and then hollow it out using a thin wall feature. Just click the thin wall icon, select the flat surface at the neck to remain open, assign a common thickness (say 0.10”) and finish.

Here the bottle is visualized with a translucent material from the style palette. 

Now let’s say that you want an addition level of realism, and want a thicker handle. Edit the definition of the thin wall, change the common thickness to 0.05”, and in the “Unique Thickness” field, select the face of the handle and assign a different thickness (say 0.10”). 

Note that the thin wall feature cannot create areas of different thickness if those areas are tangent to one another. Said another way, unique thickness areas should not be tangent to areas with a different thickness. If you need areas with different thicknesses to be tangent, create the non-tangent unique thickness thin wall first, then apply fillets to the inside and outside to transition between the different thicknesses, as shown below. 

After following the steps in Tip 11, we have arrived at the task of finding the volume of an irregular shape. There are many ways to calculate a complex volume, but here is what may be the simplest of them. Start with the container for which you want to find the volume. Add a new body and extrude a feature that completely encloses the container, up to the fill level. 

In this example, about half an inch of the bottle neck will stick out of the new feature. At this point it looks like a bottle was submerged in water and frozen.

(To simplify this, I extended the “frozen material” below the bottle to avoid the cavity created by the small indentation on the bottom of the bottle. This way the subtract function only divides the frozen material into material inside the bottle and material outside the bottle. Otherwise, there would also be a “material outside and underneath the bottle” category.)

Next, use the subtract function found under Home -> Solids -> Add Body. 

As the target, select the newly created block. As the tool, select the neck of the bottle. In the “Select Region Step” Solid Edge wants to know what material you will keep. Click “Select internal regions” and “Invert Selection.” This will pick the insides, then the outsides.
 

This process creates two bodies in the PathFinder. Right click on the first one (it should be the bottle) and toggle it to construction. 

Now, using the inspect/properties dialog, you can find the volume of liquid held by the bottle. The red material seen inside the neck of the bottle is the liquid inside. The bottle itself is counted as a construction body as you can see in the PathFinder.

By default, if you click on something in an assembly, you select a part. But sometimes, you need to select a face. You can switch the priority under the select dropdown to face or part.

Design manager helps Solid Edge users perform general document management tasks without opening the software. It can be used to move, rename, replace, preview, add comments and properties, pack and go, find where used, duplicates, reports, see the entire assembly structure and more. It is valuable and easy to use.