Wednesday, June 29, 2011

How to model a softball

Remember I promise to teach you how to create the softball? Now, here are the steps:

1. Create a semi-circle that looks like this. You can create at any plane you like because a semi-circle will result to a round shape object when you apply the Revolve feature. I dimension this semi-circle with diameter 30.5mm. Don’t forget to pin your geometry to the origin.
2. Revolve the geometric 360 degree using the Center Line on the semi-circle. The result will appear as a round shape object.


3. Now, a plane is need in certain angle so that the thread can be created at the surface of the ball. In order to create a plane with an angle, an edge or a reference line is needed. Thus, I create a construction line at the Front Plane.


4. Confirm the sketch. Then, go to Features tab and expand Reference Geometry. Select the Plane tool. In Property Manager Tab, select the Front Plane as the First Reference and then select the center line that created earlier to be the Second Reference. For the First Reference, assign the angle 35 degrees while for the Second Reference assigns the coincident.


5. Make this sketch at Plane 1 that had been created earlier. Start from origin.


6. Confirm the sketch. From isometric view, clearly the sketch was made at the origin. (It means the sketch is inside the round object!) Now, extrude the sketch so that it would be at the surface of the ball. Go to the Features Tab, Extrude Boss the sketch. Use Offset From Surface end condition for Direction 1 and select the round surface. Then, set the offset dimension to be 0.2mm.


7. The result will appear like this.


8. Then, pattern the features. Expand the linear pattern from Features Tab and select circular pattern. Then, use the center line that you make to set the angle plane to be the axis of revolution for the pattern. Set the angle to be 360 degrees and pattern the features 51 times. Use equal spacing.

9. The result would be like this. Add different color to the thread features. (Extrude Boss  and Circ Pattern)


10. Mirror the thread to the other side of the part. Use the Right Plane as Mirror Face/Plane. Select the thread features as the Features to Mirror. This is the end result after I put some rendering to this part. Well, it looks like a real ball to me! Got the ball? Got to try! Have FUN!!


Warhamni (warhamni@cadcam.com.my) a.k.a 我爱你 (i love you),she is the trainer for CADCAM training centre, SolidWorks Authorized training centre. Although she join the team late but trust me, she's good in 'playing' SolidWorks and a fast learner. She can easily answer you in no time, with her lighting speed Kawasaki.

Monday, June 27, 2011

Tutorial: 3D Curve III

My final post on 3D curve- 3D sketch.

3D Sketch is a powerful tool to create a 3D curve. But if you don’t know how to use it, this powerful tool will become difficult to use. Here I’m going to show you the way I use this tool.
How are we going to create a nice 3D sketch in this 3D environment, when we actually only viewing in 2D?  Without rotating the view, all sketches we created are creating on any of the 3 standard views. 

If you cannot imagine what I’m mention above, you can open a 3D sketch; press Crtl + 7 to change to Isometric view and sketch a curve. Then press Crtl + 5 to change to top view, you can found that the sketch in created in the front plane.



To create a 3D curve, sometimes we need some imagination. It is better if we can imagine what the curve look like in the front, top and right view. 

What I’ll do to create a 3D curve with 3D sketch is create the sketch on a standard view (Front, Top or Right) first. Then I’ll change the view to Top View to drag the point of the sketch which I create just now until I get what I want it to be on the right view.

If the curve view from top not same as what you like, you can adjust it until you feel it is perfect. Hope this tips help you on your future design. 

Happy design!

Jackson (jacksonlim@cadcam.com.my) is part of the team member who good in surfacing skill in SolidWorks. You won't believe it until you see some of the exotic cars he modeled with SolidWorks.  

Monday, June 20, 2011

Tutorial: 3D curve II

I'm back with the second method to draw a 3D curve in SolidWorks.

Refer back to the 1st 3D curve tutorial, use back the same sketch. Now extrude it with Extruded Surface , and then you will get this:

Now, open a 3D Sketch then select Intersection Curve. On the Select Entities, Select both surface and click OK.

 
Then you’ll get the black color 3D curve.


This curve can be edit by editing the 3D sketch created just now. The length can be edit by dragging the end point of the curve. If you want to edit the shape of the curve, delete the relation.

there we go, the second method to create a 3D curve. The last method, next week.

Jackson (jacksonlim@cadcam.com.my) is part of the team member who good in sufacing skill in SolidWorks. You won't believe it until you see some of the exotic cars he modeled with SolidWorks.