When you place the first view on a sheet using the View Wizard command, the sheet scale is set by default to the scale of that view, and it is associative to the view. Before placing the view, you can change the view scale using the Scale list on the command bar. This, then, becomes the sheet scale.
Views placed after the first view use the same sheet scale. This ensures that the scale of all drawing views on the sheet is consistent.
Choose Home tab→Drawing Views group→View Wizard 
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If the Create Drawing dialog box is displayed, select a drawing template with a *.dft file name extension.
If the Select Model dialog box is displayed, select a part, sheet metal, or assembly document.
Click Open.
Set options on the Drawing View Wizard Options tab as needed, and then click Next.
The options that are available depend on the type of model—part, sheet metal, or assembly—for which you are generating a drawing. Refer to Tips, below.
In the Drawing View Wizard, on the Drawing View Orientation tab, do one of the following:
Select a named view as the principal view for the drawing, and then click Finish.
Click Custom to access the Custom Orientation dialog box. Use the options at the top of the Custom Orientation window to orient the part or assembly, and then click Close.
In the Drawing View Wizard, on the Drawing View Layout tab, select any additional views you want to generate, and then click Finish.
Use the command bar options to adjust how the view or views are placed on the drawing sheet.
Example:
By default, the View Wizard calculates the best fit for the drawing views based on the model size and the sheet size. You can change the drawing view scale by:
Choosing a different scale from the Scale list.
Setting the drawing view scale to match the current sheet scale. To do this, click the Set View Scale button.
Click to specify the location of the view(s) on the sheet.
Tip:
If you select multiple model views from the Drawing View Layout page, then the View Wizard command ends when you click the drawing sheet. If you select just one view, then you can continue placing orthographic or isometric views by clicking above or below, to the right or left, or diagonally with respect to the initial view.
Drawing view captions may be turned off and on for a selected drawing view using the Drawing View Selection command bar, or the Drawing View Properties dialog box.
To display assembly material removal features in the drawing view—holes, chamfers, and cutouts—you can select the Show assembly features check box on the Drawing View Wizard Options page.
To control the display of material addition features, such as fillet welds and protrusions, you can use the options on the Display tab (Drawing View Properties dialog box). You also can define a display configuration in the assembly with material addition features hidden, then use the display configuration when placing a drawing view of the assembly.
Any time before you place the view, you can change the view layout and scale using options on the command bar.
You can attach more than one model file to a draft document.
You can create more than one view layout at a time if the view orientation you specified in the Custom Orientation dialog box is derived from a plane or face. You also can use the Custom Orientation dialog box to create a perspective drawing view.
To enhance the performance of assembly drawing views, you can clear the Show Hidden Edges and Show Edges of Hidden Parts options on the Drawing View Creation Wizard (Drawing View Options). Changing these settings only affects the current drawing view you are creating.
To apply these changes to all assembly drawing views, clear the Show Hidden Edges and Show Edges of Hidden Parts options on the Edge Display tab (Solid Edge Options dialog box). You can create a draft template file with these options cleared and use it to create all the drawing views of your assemblies without hidden lines.