Different ways to create Half Section in Drawings

Do you ever need to show HALF Section views in the drawings??

Let’s discuss various ways to create them.

Using Section View

  1. Start a new drawing and insert a view.
  2. Activate the view and insert an L shaped sketch. Using SW auto snap options start the sketch in line with the circle/arc quadrant or centre point.
  3. Click on the line and select section view on view tool bar or Insert > Drawing Views > Section or right-click on sheet > Drawing Views > Section.
  4. Click NO on the prompt window for partial section.
  5. Place the section view on appropriate location.
  6. Now right-click on section view and select Isometric Section View.
  7. You may remove the section view label if required.

    Using Configuration

  1. Open the part for which you want to create the half section.
  2. Start a new sketch on the face/plane.
  3. Create a rectangular as shown.
  4. Click on Extrude cut on feature tool bar or Insert > Cut > Extrude. You may or may not exit the sketch editor.
  5. Using any options, create the cut extrude feature.
  6. Switch to configuration manager.
  7. Add a new configuration. I have added a Cut View named configuration. And renamed the other to Full View. You can give any name as desired/required.
  8. Activate the full view configuration and switch back to feature manager. Suppress the cut extrude feature we added above.
  9. Now we have Full View and Cut View configuration with no cut and cut.
  10. Start a new drawing and place a view. Set the configuration to Cut View in case you don’t see the cut.
  11. Click on Area Hatch/Fill on Annotation toolbar or Insert > Annotations > Area Hatch/Fill or right-click on sheet > Annotations > Area Hatch/Fill
  12. Now select the threes faces produced by the cut extrude.
  13. Set the Hatch options and click OK. You may set options for individual face by selecting the face/hatch and accordingly set the hatch options.

Using Broken Out Section View

  1. Place the view and create a rectangle as shown. Make sure it passes through the centre. For easy viewing I have thickened the sketch line and colored it red.
  2. Right click on any line and select “Select Chain”. Complete rectangle will get selected.
  3. Click on Broken-out section on View layout toolbar or Insert > Drawing Views > Broken-out section or right-click on sheet > Drawing Views > Broken-out section.
  4. Specify the depth or select edge etc. to set the depth. You may select the option to see the preview when changing depths.
  5. Click OK after you have set the options.

The above options are shown for parts files only. You can also use them for assemblies.


2 thoughts on “Different ways to create Half Section in Drawings

  1. Jay

    Hi, Its interesting and useful.
    I have a query on half section. When we make the half section on center of the component, the center line of the section view will be shown as centreline line-type or the continuous line. Is there any ISO standard available for this.

    Thanks for your great help.


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