2D Drawings

To add a new 2D drawing:

1. Create a 2D drawing in the following ways:
   
   • From Export, select Drawing.
   • Go to the Add menu > Drawing.
   • From the Items Manager, select New Drawing.
   • From the Items Manager, select the item for which you want to create a 2D drawing > New Drawing...
   • Directly select the part of your body for which you want to create a 2D drawing, then from the adaptive menu, select Create Drawing.
2. Select a 3D body in the design space and then select Next.
    
   
3. in the Drawing Preferences dialog, specify the following settings:
   • Sheet Size - Following either ISO or ANSI standards.
   • Orientation - Choose between portrait or landscape.
   • View-to-Sheet Scale
   • Include Base Views - When enabled, the front, left, top, and isometric views of your design will be projected onto the sheet by default.
     
     
4. Click Continue to generate the drawing sheet.
   Note: The title block and borders of your drawing sheet are automatically generated and cannot be customized at this time.
5. You can check and adjust your sheet preferences by selecting Drawing Preferences.

You can add multiple projections of your 3D model in a 2D drawing to highlight every detail. These projections are created from different types of views: 

• Principal view
• Section view

Principal views

You can add the following basic views of this component: 

To add different views of your model, select Views in the menu and then any view from the Views toolbar.

You can move the projections anywhere in your drawing: Select the entire view and drag the arrows to reposition the projection.

If you don’t need the view anymore, double-click/tap the projection on the sheet and select Delete in the menu or press the Backspace or Delete key. 

Depending on how you want to organize your drawing, you can change the ratio of the drawing sheet to view: 

• If you’re creating a drawing from the Export menu, then you can select View-to-Sheet Scale in Drawing Preferences and set up the ratio there. 
  
  
• If you’re already working on a drawing, go to Drawing Preferences >  Sheet Preferences > Sheet Scale and tweak the ratio.   
  
  
• You can also select the View scale badge that appears when you select a projection, and then adjust the ratio.
  
  

If you want to see hidden lines, select the Hidden lines button. The hidden lines will be shown as dashed lines. To remove those hidden lines, select the button again. 

While you're working on your drawing, you can add views of different bodies, too. Select Add Bodies, then select other bodies that you want to include in your drawing. 

Section views

You can create section views from the projected principal views and visualize the interior of the model. Then, you can dimension the section views to annotate further.

Follow these steps to create section views in your 2D drawing:

1. Select Views in the menu.
   
2. Select Section.
   
   Notice that purple reference points appear on the view. 
3. Draw an imaginary line through the projection as if you're sketching a real line. This line is called the section line and it defines the plane that cuts through the object.
   Use the reference points as guides to precisely place the section line.
   If you'd like to replace the section line with a different one, simply draw a new line. The old section line will be removed automatically. 
4. Drag one of the arrows next to the section line to determine the direction of sight and place the section view onto the drawing sheet.
   Notice that the leaders, the black arrows pointing at the section line, indicate the direction of sight, and the section view is labeled with an alphabetical letter. The hatch pattern below indicates that the hatched area forms one body and they're created from solid material.
   
   Later, you can move the section view with the vertical and horizontal arrows. 

You can select from 10 types of dimensions to add to your drawing. Check out the table below to learn about each dimension type.

Add dimensions to your drawing in just a few steps:

1. Select Dimensions in the drawings menu.
   
2. Select a dimensioning tool.
3. Select the items that need to be dimensioned.
   
4. After you finish adding dimensions, select Done.
   
5. To add a prefix text, suffix text, or size tolerances to a dimension, tap the dimension, and then select the dimension editor badge.
   
   • Prefix Text - Enable to enter a prefix text for your dimension. For easy access, you can select any of the commonly used symbols available in the Prefix text field below.
   • Tolerances - Enable to enter a size tolerance applicable to your dimension. To choose a tolerance type, select the drop-down menu and choose between Symmetrical, Deviation, Limits, and Basic.
   • Suffix Text - Enable to enter a suffix text for your dimension. For easy access, you can select any of the available commonly used symbols below the Suffix text field.
     
6. Optional: Drag the dimension on the sheet to reposition it anywhere you want.
   
7. If you want to remove a dimension, tap it and then select Delete.
   

Note: You can directly select a line, curve, or any other item in your drawing. The adaptive interface will automatically dimension the item and you can confirm it by selecting the check mark or pressing the Return key.

If you select items in a view, the menu is customized automatically. From the adaptive menu, you can select the appropriate tool to instantly dimension the selected items. If there is only one dimension possible, the dimension is automatically applied.

To specify the precise decimal measurement of Linear and Angular dimensions, select the Drawing Preferences settings icon from the top right corner then look for Dimension Precision.

You can annotate parts of your drawing with the Notes feature. 

1. Open your 2D drawing. 
2. Select Text. 
   
   
3. Select Note. 
   
   
4. Select a line or curve.
   A text box will appear, and you can type or write your notes. The character limit is 1,200.
   
   
5. You can drag and drop the notes anywhere you want.
   
   
6. Select Done to exit the tool and finalize the annotation. 

If you need to edit the annotation, double-tap or double-click the text. An editable text box will appear. You can always delete the annotation by selecting it and pressing the Backspace or Delete key, or selecting Delete. 

You can annotate the non-isometric views in 2D drawings with geometries. Shapr3D supports the following geometry types:

• 2-point centerline
• 2-line centerline
• 2-point circular centerline
• 3-point circular centerline
• Center mark
• Intersection mark

Centerline

Centerlines are dashed lines that run between two reference points or lines. You can use them in 2D drawings to: 

• Show the axes of circular or cylindrical features such as holes and discs
• Dimension circular features
• Point out features that share the same central axis

Note: Centerlines can’t be dimensioned with the Line length tool.

To add a centerline, follow these steps:  

1. Select Geometries in the menu.  
2. Select one of the geometry tools: 2-Point Centerline, 2-Line Centerline, 3-Point Circular Centerline, or 3-Point Centerline. 
   
   
   
3. If you chose 2-Point Centerline or 2-Point Circular Centerline, select two points as reference in the drawing.
   
   

   2-Point Centerline

   2-Point Circular Centerline

   
   If you chose 3-Point Circular Centerline, select three points on a circumference. 
   
   
   If you chose 2-Line Centerline, select two linear lines as reference in the drawing.
   
   
   
   A centerline will be created between the reference points or lines. 
4. Extend the centerlines by dragging the arrows.
   
   
   
5. Select Done to exit the tool and finalize the geometries.

Center mark

Center marks are cross-shaped annotations that indicate the centers of circles, arcs, and circular edges. You can also mark these centers as reference points for dimensioning. 

To add a center mark, follow these steps: 

1. Go to Geometries > Center Mark in the menu. 
2. Select the center of circular edges.
   
   
3. Select Done to exit the tool and finalize the geometries.

Intersection mark

Intersection marks are cross-shaped annotations that indicate where two non-parallel, linear lines intersect. You can also mark these points as references for dimensioning. 

To add an intersection mark, follow these steps: 

1. Go to Geometries > Intersection Mark in the menu. 
2. Select two linear lines that are not parallel. 
   
   
3. Select Done to exit the tool and finalize the geometries.