How to change the blades on a 'dumb solid' (CATIA)

Jack K

15 Oct, 2018 02:02 AM

This tutorial is to provide a guide for modifying a CATIA file containing a "dumb" solid.

(The reader should be familiar with basic CATIA Part Design commands)

This tutorial is to respond to a recent question asked by Nouman Khalid:
"This dump solid is generated from a STL and i am given a .STP file. I want all the blades to be similar to generate a reference model for modal analysis. I want the encircled blade to be copied all over rotor. Please guide how this can be done."

1. Step 1: duplicate the fan

   a. Copy the Body

   b. Paste Special into the Part file using the AS RESULT option

   c. the result will be a second Body that is identical to the first

2. Step 2: rename the Bodies

   a. rename the first Body as "Center Hub"

   b. rename the second Body as "Propeller Blades"

   c. Hide the Propeller Blades Body, so only the Center Hub body is shown

3. Step 3: modifying the Center Hub

   a. right-click on the Center Hub Body and choose the Define As Work Object

   b. create a new sketch on the front face of the hub, and draw a circle the same size as the hub OD. (either measure the diameter first and add a dimensional constraint, or project the outside edge of the hub onto the sketch)

   c. use the sketch to add a Pocket passing all the way through the part. Make sure the red arrow is pointing out of the circle to remove all the blades. Only the hub should remain

   d. Hide the Center Hub body

4. Step 4: modifying the propeller blades

   a. Hide the Center Hub body, and Show the Propeller Blades body (you should see the entire part again)

   b. right-click on the Propeller Blades body and choose Define As Work Object

   c. create a new sketch on the face of the hub

   d. rotate the sketch normal to the screen, and sketch a polygon around one of the blades. It's OK if the polygon is a little inside the OD of the hub, but it should be totally outside the one blade

   e. use this sketch to add another Pocket passing all the way through the part. Make sure the red arrow is pointing out of the polygon to remove all but one of the blades. Only the one blade should remain

   f. add a Circular Pattern to duplicate the blade around the center axis (Z-axis?) of the part. Add as many blades as required

   g. Show the Center Hub body so both bodies are seen

5. Step 5: Combine both bodies

   a. Make the top body the Define As Work Object

   b. right-click on the other body, and choose the Boolean Add option

   c. add fillets where the blades meet the center hub

   d. save the modified model as a new CATPart file