The results of the Create 3D command vary depending upon the model type and whether it contains synchronous objects, ordered objects, or both. See Finishing the sketches to learn more.
Select the Tools tab→Assistants group→Create 3D 
.
In the Create 3D dialog box, do either of the following:
(To create a new model file):
Select the Add to new file option.
From the File list, select a template for the model you want to create.
(To update a model file):
Select the Add to existing file option.
Use the Browse button to locate and select the assembly, part, or sheet metal file you want to update.
Click Next.
To define the primary (first) sketch view, do all of the following:
In the Create 3D dialog box, under View Properties:
Select Fold principal views.
From the Primary view list, select the view orientation you want to create (front, back, right, left, top, or bottom).
On the drawing, select the 2D elements to define the primary view orientation. You can drag a box around the elements to include, or press the Shift key and click each element.
To include dimensions in the sketch, you must also select them in the drawing view.
To define another view, click the Next button and select the elements to include.
Tip:
You can use the Fold principal views, Fold auxiliary views, or Copy view(s) options to define additional sketches. See Selecting view types.
Repeat the previous step until you have defined all of the required sketches.
Click the Finish button.
This opens the model document with all of the sketches placed in it.
(Optional) Use the 3D steering wheel to adjust the position of the sketches and associated PMI dimensions in the model document:
In PathFinder, right-click the Create 3D user-defined set that contains the sketch you want to move. To move all of the sketches as a group, right-click the last Create 3D user-defined set in the list.
Reorient the steering wheel to move the sketches and associated dimensions.
When the sketches are positioned correctly, right-click the user-defined set again and choose Attach PMI.
See Working with Create 3D user-defined sets and Moving PMI dimensions created by Create 3D to learn more.
Tip:
After you select the geometry for the second view, you can click the Set Fold Line button to define a line or point in an orthogonal or auxiliary view about which to fold the view. This insures proper orientation of the sketches.
To learn how, see Defining a folding line.
You can change the Scale value for the model geometry created from each drawing view.
You can click the Options button to change the default setting for drawing view projection angle, and to specify the dimension types you want to be able to include in the sketch.
The environment setting for opening part and sheet metal documents (on the Helpers page (Solid Edge Options dialog box) determines the default settings for creating a new file using the Create 3D dialog box.