Just another fun with the SolidWorks animation. This one talks more on in-context modeling approach and how to use that for animation. Though more focus will be on creating the animation but yes there is small though most important role of in-context modeling.
Preparing for the animation:
1. To start, create a spherical ball of any dia and the save the part as Ball ( I have taken the dia as 3in).
2. Start a new assembly and save it with any desired name and preferred location.
3. Insert a new part via Insert > Component > New part*.
4. Select front plane as the base plane for new part. You may choose a different plane too.
5. Create a sketch on as shown in the pic (you may choose different values for the dimensions).
6. Using revolve feature, create a cylinder and finally exit the part edit mode. You may save the part internally or externally as desired.
7. Now insert the ball part (created in step 1) into the assembly. Place it any where in the assembly and make sure it is floating i.e. not fixed.
8. Add two coincident mates (between front planes of ball and assembly and similarly between top planes of ball and assembly).
9. Add a 1.6in value distance mate between right planes of ball and assembly.
10. Now switch to part edit mode and edit the long tube/pipe (created through steps 3-6). You can right click on the part in graphics or in the feature manager and select edit part.
11. Start a new sketch on the front plane of the pipe.
12. Expand the feature tree for ball part and select the sketch used to create the ball.
13. Click on convert entities. This will copy the sketch used for ball onto the front plane of the pipe
14. Using horizontal line as centre line, create a revolved feature.
15. Hide ball part for easy selection and further feature addition/editing. Right click on the ball part and select hide components.
16. Add a fillet of 0.25in as shown.
17. Add a shell feature with 0.1in as wall thickness, shell outward and select both the ends of the tube under faces to remove.
18. Create another sketch on the front plane of the pipe (as shown) and do a revolve cut.
19. Exit part edit mode. And finally save the assembly.
You have finished with doing the required steps prior to animation.
* If you are using SW2007, then you’ll have to save the part externally but in higher versions, you can save the part internally in the assembly. Check SolidWorks help for more details on it.
Creating the animation:
1. Switch to motion manger/study. Set the view orientation as required.
2. Drag the timebar to any time value (I have set it to 10 seconds).
3. Now double click on the distance mate mate. This will highlight the distance value and dimension modify window will pop up.
4. Key the desired value (I have used 13.5in) and click OK to finish distance modifications.
5. Now hit calculate and then finally you can play/save your animation. Check the video under My Videos section.
Enjoy playing motion with different shapes/sizes.