In this post, we will look at the creating an impeller blade in CATIA.
The approach that we will use is using helix function, creating a surface using the helical profile and lastly making it solid using part design.
1) First, go to part design function in CATIA.
2) Then, go to the sketch function
, and click the xy plane in the specification tree.
3) Create a circle with diameter 80mm and exit workbench
.
4) Click the pad icon
. In the pad definition window, specify length 8mm and click OK.
5) Click on the surface of the newly created cylinder.
6) After that, create a circle with diameter 15mm at the center of the cylinder. Pad the newly created circle to a 25mm in length.
7) Sketch using the surface of the cylinder (above picture) as support. Select the “Point by Clicking”
. After that, make a point and have it to be coincidence with the edge of the circle.
8) Go to Generative Shape Design Module from Start -> Shape -> Generative Shape Design.
9) Then, click on Helix function, and click the point created on step (7).
10) Helix curve definition window, select these parameters:
- Helix Type: Height and Pitch
- Pitch: 200mm
- Height: 25mm
- Axis: Z Axis (Right click on the box beside Axis for the drop down to show)
11) For this step, go to Sketch and click on the surface of the small cylinder as above. Then, same as step 6, make a point coincident to the edge of the small cylinder.
12) In this step, do the same as Step 11 but use a different support this time (Click on the surface at the bottom as show in picture) and create another point.
13) After that, the result that we got after the two steps can be observed as picture above. Dont worry about the dimensions of the points as we can edit those later on.
14) Then, Create a line between the two points in step 11 and 12 by using line. Click line and click the two points to create the line. You should get the result as above picture.
15) Next, we will create a line to connect the two profiles. Refer to picture above (Left), click the line icon, then click the two points labeled as (2) and (3). You should get the result the same as the picture above (Right)
16) Use multi section solid to connect all of the lines. 
17) Take the horizontal profile as section and vertical ones as profile
18) Use thickness function in the part design workbench to convert the surface into a solid.
19) Use the circular pattern
in the part design workbench to pattern the solid from the thickness just now.
- Choose Complete Crown as the parameters.
- Instances in this example is 9, but feel free to experiment with any numbers.
- Reference Element: Use the circular cylinder surface.
20) That should be the end of this tutorial.