Attempting to align a body in two dimensions with sketch coordinates

[mmullins79KBL4]

Hi. I'm brand new and am trying to recreate my own Raspberry Pi model mostly to learn and get used to the 360 package. I'm mostly an Eagle user with some Blender experience and no formal CAD package experience.

I would like to align a body representing a header pin to the hole centers depicted on a sketch located in the XZ plane. Moving point-to-point causes the body to align in three dimensions as the screencast shows. Is there a way to constrain the movement to two dimensions in this case? If not, can you recommend a better workflow to do the same thing?

Thanks

[etfrench]

Joints are the preferred way of doing this. In the Support & Learning section of this site watch the Assembly video.

[mmullins79KBL4]

Thanks for the reply. I'm trying to get my mental model aligned here; correct me if I'm mistaken about anything.

I cast every header pin and the standoff into a component. Then I projected the appropriate sketch points onto the top surface of the standoff and joined each pin to their appropriate points.

Given my understanding of the expected distributed workflow, I selected all 40 pins and the standoff (all just simple boxes) and saved them into a separate design. Then I deleted the original components and inserted the header from the newly saved design back into the RPI design, creating a linked assembly. The final bit looks like this:

I think that's correct from what I gathered on the tutorial videos. However I have a follow-up question. Even given the intended distributed design method, what if I'm absolutely positively sure I will never reuse an assembly but still want to have some kind of subassembly in the current design? Do I still have to save externally, re-import, and then break the assembly link?

[etfrench]

There's no need to export a component, then re-import it.  The only time this is useful is when you're using the part in multiple projects.

See also Rule#1

[mmullins79KBL4]

Ok, now I'm confused.

Should I be treating this header as a component or an assembly? I'm used to thinking literally that this part is a component (plastic and brass), but to work in this context I assume it should be an assembly, not a single component. You also told me earlier that it would be best to attach the pins using joints. That implies that each of the pins should be its own component and that the components together, the whole header, should be an assembly. And the only way I can figure out to create an assembly is to do so by working in an external design.

[davebYYPCU]

Yes it is confusing, because there are many ways to skin the cat, 

so look to your end game, what do you need in the end, and work towards that.

To use the header set, in future projects, yep save it as a component.  When inserting, can be placed with point to point in the insert process called the free move, and locked with rigid group to the circuit board.

Without the file and a stated end game, we have to guess the answers you are looking for.

Might help....

[etfrench · Accepted solution]

I don't think there is an actual definition of an assembly.  It's just a collection of components with the same parent. 

Here's how I would create the header:

1. Create new component called Header.
2. Create sketch for the top view of the header.
3. Draw outline of plastic with length and width parameters using formulas based on the number of pins.
4. Draw the outline of one pin. Use dimensions to locate it.
5. Extrude the plastic portion as a new component.  It should be created as a sub-component of the Header component.
6. Extrude the pin as a new component under the Header component.
7. Use a rectangular pattern to create all of the pins. If you use the pin body instead of the pin component, all of the pins will be created under the pin component.
8. If a joint origin doesn't exist at the center of pin 1 where it meets the plastic, create one.

[mmullins79KBL4]

etfrench,

Ah hah.

Point 5 is the key thing I wasn't understanding. I didn't realize you could create subcomponents within the active component. I'm sure that's obvious and I'm being pretty thick, but newbies are called that for a reason. And I'll mark that as the answer. For reference, I was looking at these videos:

http://help.autodesk.com/view/fusion360/ENU/?learn=assemble

And took the process as gospel. Thanks for the link to Rule 1 as well; I'll do so in the future.

If you're willing I'd like to poke at the answer some because the primary objective, as davebYYPCU asked, is to for me to make and correct mental models. So say I have a whole bunch of components that I want to group together and treat as one thing. I don't need to share or use it in multiple projects. What would you do? The reason I ask is because what you said in point 5 is probably the best way of going about making components inside other components, but what if I screwed up my planning and have many disparate components that need to be grouped together into a single component?

[etfrench]

You can use rigid groups or rigid joints to ensure components or bodies stay together.