 |
| Tools from Views toolbar |
If you are starting from scratch. i.e. you have no views on the sheet and have only set the drawing sheet. In this case, the first view that you should create is the front view.
Front view
After selecting the tool, go to the part / assembly window for which you wish to create the view and select a plane of your preference, based on which you wish to create the view. You would be able to manipulate the view using the blue tool that appears on the top right corner.
 |
| Creating front view |
As soon as you click somewhere on the sheet, or in the middle of the blue tool, the view will be created. When you have a view on the sheet, and that view is selected (you can select a view by double clicking), a whole set of other tools will also become active, and you would then be able to use other set of tools too from the views toolbar.
Advanced front view
The advanced front view works in the same way, as the front view. However, in this case, after you select the tool, you get the option to define a scale of the view. So, you can set this value and the view will be according to the scale and not according to the one you set during the sheet setup.
You can use this in case you want to create an enlarged or reduced view. After defining the scale, you need to go to the part / assembly window and select the plane of reference as you did in case of the front view.
Projection view
Based on the angle of projection set for the sheet, you would be able to extract and place right / left / top / bottom view using projection tool. The tool will work only if some view is selected. To select a view, you can double click that particular view, it will highlight the view and the bounding box will become red, indicating that it is selected. Subsequently select the tool, and move the cursor in the direction of the view you want.
 |
| Using projection to extract views from active view |
For example, in case of third angle projection method, if you move the cursor to top of the front view, preview of the top view will be shown, and if you move it to the right of the view, the right view preview will be shown etc. The view will be created as soon as you click somewhere on the sheet, keeping in mind the preview that is being shown at that moment. You can use this step repeatedly to create any view you like. Also, you can select any view and project it using the projection tool. Views will be named as per the view from which you extract the view.
Unfolded view
All sheet-metal parts are essentially manufactured by forming flat sheet-metal rolls. So to manufacture, it's important to find out what would be the shape of the sheet metal form before it undergoes any of the manufacturing processes. Such an unfolded view, will reveal where are the bend lines and how we are to proceed with the forming process. To extract information about the unformed part while it is in flat shape, we used the unfolded view. Since we have not studied the sheet-metal design yet, we will skip this tool.
View from 3D
We have a specific workbench for creating annotation and functional tolerancing of the part. In this workbench, we can add specific permanent views in the specification tree for quick analysis of part in the 3D environment itself, and we may bring these views also into the drafting workbench using view from 3D tool.
 |
| View from 3D |
If you have created any such view, you can use the tool to bring the view in drafting and apply dimensions, annotative text, tolerancing of such key sections / views etc.
Isometric view
An isometric view can be used to insert any particular view from the 3D environment. You can orient the part in the way you prefer. After selecting the tool, navigate to the part window, adjust the part view in the way you prefer and to generate the view, click anywhere on the part. It will generate that view and take you to drafting workbench where you can place it with a click.
 |
| Generating Isometric view |
Within the drafting workbench, you can move in any way possible and place it wherever on the sheet.
Auxiliary view
Any view on the drawing sheet can be used to generate an auxiliary view. To do this, you need to select that view. Subsequently, after selecting the tool, click on the screen to define the first and second second point of a line.
 |
| Generating auxiliary view from Isometric view |
This line is basically the viewing direction, using which the auxiliary view can be generated. You can also edit this view by double clicking on the same line and modify viewing direction and line placement.
Offset section view and Offset section cut
An offset section view is a flexible way of creating section views. Not only can you use this for creating normal section view, i.e. a section with single plane, but also an offset section view. To create a normal section view, you would use only one line. However, if you wish to create a section view, that's offset by some distance, you can use this same tool. The way to do it is that you keep making line with clicking points and moving the mouse cursor, and when you wish to end, you can do so with double click and the view will be created.
 |
| Difference between offset section view and offset section cut |
The offset section cut is created in the same manner. However, the difference between the two is that in offset section cut, only where the plane cuts the part is shown, in case of section view, the part view is also shown along with the section cut.
Aligned section view and Aligned section cut
Offset section view, even though cut the part using different planes, the planes are essentially parallel to each other. Now, in case you wish to create a section using non parallel planes, you can do so using aligned section view / cut. In this case the aligned section is imagined to be rotated about the centre, and oriented the same as the original plane.
 |
| Creating aligned section view and cut |
This is the kind of view that you are most likely to create in case of circular components or angled parts where you wish to show section in one view itself. Difference between the aligned section view and aligned section cut is the same as we studied in offset section and cut. Above you can see it applied to an assembly of plate and bolts.