Help with Cylinder Plate Design

[ehrenbeck]

Hi,

I am trying to model this cylinder plate and then create a file from which I can then machine it on my CNC mill. I am a complete beginner in CAD, but was able to make some pretty good progress. The only trouble I am having now is completing the 5.0 mm contours on the ends. I tried drawing a 5.0 mm arc from one of the "ears" but I dont know how to cut that part out of the body. Any help would be greatly appreciated!

[Mike.Zhang · Accepted solution]

Before give you some detail steps about how to make it, I'd like to give you some tips to finish this kind of model.

1. It'll be more easier if you draw all the profiles in only one sketch before you use Extrude or other model tools to make it.

2.In current model, you can create a new sketch, and create all the profile you need base on the position of current sketchs/solid model.

[Mike.Zhang · Accepted solution]

Here comes the detail guidline.

1. Use the picture you have as the Attached Canvas, then use it as reference in sketch creating.

 

2.Adjust the size of the canvas, make it approximate to the real size

3. Change the Opacity of the canvas, make the sketch more obvious

4. After analyzed the part, found it's a symmetry part, we can just create one quater of the whole profile, then use Mirror Command to create the left parts of the whole profile.

--- Create the two center lines as reference base on the canvas. (Tips: We can use Normal/Constrution option to change the line types)

5. Create top left corner circles and set the dimensions base on the canvas

6. Add the two 3-Point Arc on the two circles, maybe this is the pain point of you, so I'll decribe it in details

7. Press Ctrl key, then select the two center points of the circles, right mouse click, select "Fix/Unfix" command to fix the circles, so they will not move when we add constraints.

8. Invoke Constaints command, select the Tangent option, then click the arc & circles you want them keep tangent, then got below result.

9. Set the dimensions of the arc as R5.0 by using Sketch Dimension command

[Mike.Zhang · Accepted solution]

10. Add the straight line in the center position, set the dimension.

11. Invoke Sketch Mirror command, select the circles, arcs and the lines as Objects, then click on the horizontal line as Mirror Line, OK, got the left part.

12. Use Sketch Trim command to delete the curves we don't need.

13. Use Sketch Mirror command again to get the right part of the profile.

14. Invoke Model Extrude command, select the profile we got, input the distance, OK, then got the solid part.

[Oceanconcepts]

Mike, I just want to say that you have done a great job of explaining an area that is a stumbling block to those new to CAD- I hope this sort of thing can be archived in the learning area as a tutorial on sketching.

[Mike.Zhang]

Ron, Thanks your suggestion!

We'll consider to add some good replies into the learning materials.

Regards,

Mike