How can I create a piping library part. It is the creation of
the CPoint and RPoint that gets me. When I drag and drop a 90 bend
from the piping library, it is a sldprt file and it has 2 cpoints
and 1 rpoint in it. How do I create a part file that has the
required points in them.
As far as I can see, they are only avavilabe in an assembly. Lets start with something very, very basic. Draw a circle and extrude it to a solid. Let us call this masterfull piece of engineering a valve. Create a new sketch and place 2 Points at the centre faces of the valve ( these will be used for the CPoints and RPoint later on). Save the part. The next part is the problem. How do I place CPoints and RPoints on the points created on the previous sketch??
I know once the CPoints andRPoints are there, you do some design table stuff with Diameter@CPointn etc, but I cannot creat the CPoints in the first place.
Can someone show me how to do this? Any Help would be greatly appreciated.
Thanks
Stu
As far as I can see, they are only avavilabe in an assembly. Lets start with something very, very basic. Draw a circle and extrude it to a solid. Let us call this masterfull piece of engineering a valve. Create a new sketch and place 2 Points at the centre faces of the valve ( these will be used for the CPoints and RPoint later on). Save the part. The next part is the problem. How do I place CPoints and RPoints on the points created on the previous sketch??
I know once the CPoints andRPoints are there, you do some design table stuff with Diameter@CPointn etc, but I cannot creat the CPoints in the first place.
Can someone show me how to do this? Any Help would be greatly appreciated.
Thanks
Stu
When I see your questions I feel like Donkey from Shrek "Where do I start?"
That would be much fun to start everything from scratch. Make all library parts nice and right.
First advice. Valves. You start valve. The simple one. Make it right. All other valves will be made off that one. It will be your template for all others. This way Replace Components Option will work smooth and easy when you will need to replace valves.
Sample: Ball valve Jamesburry. Steel body. (We keep manufacture name in part name just as reference to dimensions that were used in part design). It will be SW/Threaded. Flanged could be made as separate part.
1. ½" valve. Start from smaller size. It's easier to go from small to big when you add configurations later. Built cylinder-body-extrude as you said. On Front Plane. Circle-extrude mid plane. So the middle of valve will be at origin. Always.
2. make cut where your pipe/nipple will be inserted. On one of the faces. Use correct depth - for thread/socket cut. It's important. How much nipple will go inside valve. Mirror cut to other face.
3. Make handle on top. All the sketches fully defined (black color, nothing blue allowed). Name features properly (body, pipe depth, handle). When you built features consider what could be suppressed in future. Try to avoid dependence off features that could be suppressed in other configurations. Try to make them in such fashion that double-click on feature will give you only dimensions to modify by design table. (valve handle height)
4. Avoid fillets and chamfers. DO NOT use them in design. They make files heavy. On drawings they will create unnecessary lines. Part will look thick. Sometimes just black fat spot instead of little valve. They are not good features to have for mating as well. Make parts as simple as possible. Fancy parts good for advertisement. They don't look professional.
5. Now. When you done with part. Select Side Plane (CL) - sketch on it three dots. Two C (with relations in middle of pipe depth cut and R at origin. Exit sketch.
6. View-Toolbars-Routing Tools. Click C-point button (line and dot on end). Give properties for your piping in Connection Point window on left of screen. See attached picture. Do R-point in same manner.
7. Add valve configurations