What is it exactly that you are trying to do?
Are you trying to setup equations for the layout sketch to control the location of the parts? Or are you trying to control the size of the part based on dimensions from the assembly?
I am probably trying to do both,There is an example posted by Mauricio Martenez-Saez (door on frame) I tried to put a link in but couldn't, but basically he has drawn a door frame and door and linked the values of dimensions with equations, I can find the equations but cannot find how, or where he put the links in.
Sorry but I have no experience of linking dimensions between different parts and do not know how to go about it.
Help would be appreciated.
Sorry it took me so long to respond again, I've had a pretty busy couple of weeks.
I've taken a look at the "Door on Frame" example you pointed me to. Here's what I see in the assembly (hopefully this helps):
- He drew a sketch in the assembly as a layout sketch.
- He created parts "in-context" and referenced the layout sketch using relations and equations. In case you've never created a part in-context before, here's how you do it:
- Click Insert -> Component -> New Part
- Click on the Plane on which you would like to start sketching. Note, you will be automatically entered into a sketch on the plane that you selected, but you don't have to start sketching on this. You will be editing the part in context, so you can exit the sketch and start a new one on any plane you wish.
- Start drawing sketches and creating features as if you would normally create the part, except that you can create relations to the layout sketch in the assembly. Do this just like normal, for example, select a point on the sketch you are drawing in the "in-context" part and then select the point on the layout sketch, then click the "Coincident" relation. That relation is now related to the layout sketch and the part will modify according to any changes in the layout sketch. This is how the door frame is made, the door has some special quirks in it (see below).
- To get out, right click in space and hit the "Edit Assembly: Door on Frame" option.
- The door is a little bit different because it isn't fully defined and includes equations. In order to achieve this, create a new part in context and then create the features (in the case of the door it is simply an extrude). Then do the following:
- Return to editing the assembly (Right click in space and click "Edit Assembly: Door on Frame".
- Delete the InPlace mate that was created for the door frame, then mate the part where you want to.
- In the case of the door, 3 mates were performed. (1) mate bottom of door to top plane, (2) mate corner of door to rotation axis, and (3) a limit angle mate.
- Notice that two dimensions in the assembly file were named, Door-Thickness@Sketch2 and Door-W@Sketch1. Edit the door part (right click the door and click the "Edit Part" button).
- Click Tools -> Equations -> Add
- If you see the width dimensions of the door, click it to add it to the equation, otherwise, click the door and then click the width dimension, then type =
- Add the following to the equation, Door-W@Sketch1@Door on Frame.SLDASM (including the quotation marks). I don't think you can simply click on the assembly equations in order to get the name in the equations, you have to actually type it in. The general syntax for referencing dimensions in the assembly is "Dimension Name@Sketch Name@Assembly File Name.SLDASM".
- Click OK, then do the same for the door thickness (Door-Thickness@Sketch2@Door on Frame.SLDASM)
- Get out of editing the part.
That should be it. Hopefully this helps. If there's anything else that I've missed please post a note and I'll try to elaborate.
Thanks for a very comprehensive answer, am working my way through reproducing "door on frame" and have made some progress, am having many problems but will post them only when I have exhausted try,trying again.
Feel free to ask anything anytime... there are lots of great people on here who are always very willing to help.