Possibilities of SolidWorks

Well, yes, SW can make parts associative to one another in an assembly or in just the part environment. Yes, SW can do boolean operations. Yes, SW can make blocks with holes as well as cylinders.

The best suggestion I think is to go get a 30 day trial or sit in a SW reseller's office to use the product to see if it does what you want. I think in the end you'll see that SW does it, but would handle it better if you change the way you do things a little.

Good luck,

Matt

Riverdeep wrote:

Thank you for your advice. Of course I know that SW can manage associative operations. Of course I know that SW can make blocks with holes!!

My example was only a simplification of a complex design process. What's interesting is how do you get from Part1 to Part4. How do you make the points of Part1 to be the beginning of Part2 with retained associativity? How do you manage assembly (or whatever) to create Part4?

Is "derived part" or "mold design" applicable?

From your question, it was hard to tell what you know, if anything, about SW. What you asked about is a very basic process, unless I'm missing something important.

The best way to do specifically what you ask is to put part 1 and part 2 in an assembly. I would assume you would edit part 2 in the assembly and draw 4 lines such that the points in part1 correspond to the endpoints of the lines. That assumes that you have a plane to sketch on or don't mind using a 3D sketch. If you don't have a plane, planes are easy to create. It also assumes that the 4 points are coplanar, although technically it doesn't have to be that way. Anyway, once you have the 4 lines forming a closed loop you can extrude a block inside part2, associative to the points in part1 being edited in the context of the assembly. If the points in part1 move, and the assembly and part 2 are open, part 2 will update. Whether part2 gives an error or not will depend on how the points are moved. If the points move in such a way to make the lines in part 2 overlap, touch at a point, cross themselves or become zero length, the solid will no longer be created.

You can use sketch relations to draw a circle to extrude or a rectangle to revolve for the cylinder in part 3 using the same in-context technique.

To boolean part 4, you could use either an assembly or a single part. If a single part, you would use Insert > Part to put both parts 2 and 3 into part 4 and use the Combine command. Or you could just insert part

2 directly into part 3 or vice versa. If an assembly, you would edit part 4 in an assembly, use Join to bring part 2 into part 4, and then use Cavity to cut part 4 with part 3.

Since the first part is just sketch geometry you would insert it into an assembly and the second part would be modeled in context from the first. The third part would be dropped into the assembly and and a cavity performed on the second part to get to part 4.

In this example an assembly would provide the relationships between the various parts and would have to be open when the associativity is expected to hold.

The way you worded your original post makes me wonder if you are an I-Deas user, as it's reference geometry capability is much better than Solidworks' (at least at 2004 that I'm on).

I don't know if the later versions are better, but at 2004 you can't add reference points at a series of dimension-driven x,y,z absolute co-ords, or relative to another reference co-ord system.

You also can only create a reference co-ord system by defining the origin and a direction for each of the axes i.e. no angle dimensions driving the plane definitions, no polar co-ord systems.

Regards, John H

Thank you Matt, Top and John. I have learnt a lot from your postings and is confident that SW will do for my purposes. Yes, I have a long experience of I-deas. But I was thinking in terms of ProE when I formulated the problem.