Assembly drawing techniques to use reference geometry

[ksumet92]

We manufacture products that consist of many sub assemblies compiled to create a top level product. We would like to provide MFG. assembly drawings that show how these subassemblies are assembled and how they assemble to the base (next level up) assemblies. That is, we need reference geometry of surrounding parts and components but don't want them in the assembly we are detailing.







A simple example: We have a subassembly that is a grouping of decals. These decals get placed on a machine. We need to create a drawing that shows how and where the decals get placed on the machine. What methods have been used?







Thanks,







Steve

[harco]

In your model RMB on any assemblies you want as reference only and set the BOM structure to reference this will remove them from the BOM but they will be visible.
When you place the view in a drawing the reference parts will come in as phantom lines only enough to show connection with the true parts.
If you wish to show the reference parts as full lines then edit drawing view> model state and set reference data line style as parts.
Hope this helps.

[ksumet92]

Therefore you would use the top level assembly in the drawing, not the sub assembly model itself, then show the BOM and parts you want to use. OK. Does this process work for multiple occasions? In my example, the top level model is in reality a collection of app 100 options. Does it work to do this multiple times in the top level model?

Thanks for the input.

[ljapsey]

Well.....what a great little tidbit of information for controlling the linetype of referenced models. Learn something new everyday!

Thanks, Larry

[harco]

It really depends what you want to get out of the drawing the way you set it up.

Say you made trailer towbars for cars and you had 10 models of towbar, you don't make cars but you do have Inventor models of them.

You would make up your towbar assembly in Inventor with all the parts set to normal then place your car model in that assembly and set it to reference.

Or if you wish to show the towbar as a complete assembly you could make a higher assembly with the towbar normal and the car again at reference.

If you want to show numerous optional towbars on one assembly drawing this could be possible using view reps but all the towbars will show on the BOM.

I would think it would be simpler to show each option on it's own drawing as each assembly needs to be constructed anyway.

Level of detail is another option, I haven't really used it so I can't comment much but many lads on this newsgroup do use it and they seem to get the functionality they want out of it. I think it's a way to control the BOM view where all the parts are normal but you may not want then all to show in one view, don't quote me though.

I would say that if you want to show all the options on the BOM but have separate drawing views of the assemblies in place where referenced then view reps & referenced parts should give you that. It may get messy though if you want to put everything into one top assembly.


A bit more in the right direction but not much!!:)

[signmeup]

Is there a way to make the whole reference component show in the drawing view? It seems to be up to Inventor as to how much it shows. You would think this could be controlled by the crop feature if people don't want the whole thing showing.

[SBix26]

Edit the view, then set the Margin to larger values.  This works well most of the time, but the margin is calculated based on the center of the non-reference stuff in the view, so occasionally it shows much more of one reference part that I don't care about in order to display all of one that I do care about.