One drawing to make multiple parts?

[KirbyWan]

Howdy all,

I'm creating 3D models of some aircraft panels. These panels are all gently curved in only one direction. They consist of an outer skin, three doublers on one side and three doublers on the other side that mate up with a small gap, some core, an inner skin and a few other little parts.

I would like to (and have) create a drawing with all the part edges in one sketch, and then just extrude the regions needed for each part. I've done this, but by creating the sketch and then copying it into each part number as needed. Now if I need to make a change I need to make it to each sketch individually.

Is there a way to use one sketch that controls all the parts? That way if I want to move a tooling hole to adjust the fit I make it once and it propagates to every skin piece.

Thanks,

-Kirby

Using SolidWorks 2010.

Kirby Wilkerson

Remember, first define the problem, then solve it.

 

[CorBlimeyLimey]

One way is to create a part consisting only of the controlling sketch, and then insert that part as the first feature of the actual parts. The geometry of the actual parts should then reference the controlling sketch. Any changes to the controlling sketch will be reflected in all parts referencing it.

 

[Eltron]

Yep. That's a classic example of top-down design. Look in the help for "envelope" or "skeleton" parts.

Dan

http://www.eltronresearch.com

Dan's Blog

 

[Gurjjeet]

Apart from what CBL mentioned....

1.Another way can be to draw the sketch in an Blank Assembly file & then insert new parts (with same reference planes)& use the sketch to convert entities into your part sketches.

2.Another way is to just create one part file with diffrent parts as bodies & then save those bodies as parts(by right clicking on the body in feature manager.

As you mentioned they are overlapping part.......I guess they do not move in relation to each other.........in that case method 1 is best suited.

Hope that helps....

 

[KirbyWan]

O.K. I was giving this a try and I've run into problems. Perhaps I'm missing something. I created the sketch and saved it as sketchonly.SLDPRT. I then create a new part and click Insert -> Part and insert the part and nothing is there. If I go into the sketch and extrude some part of the sektch it imports this extruded part but with no refereence to the original sketch. I did a search on skeleton and came up with nothing. I searched for envelope and wasn't sure anything was relevant. I've included one of the simpler panels I'm working on. For each part I would select the contours I want extruded. This part has one outer skin, three doublers on each side of the part, two pieces of beveled honeycomb core and two inner skins and the beveled core use fiberglass to closeout core edge. So I would make 9 parts from this sketch and possible templates for cutting fiberglass locating the core and a caul plate.

-Kirby

Kirby Wilkerson

Remember, first define the problem, then solve it.

 

[Gurjjeet]

Hello Kirby

I cannot open your file as I donot wanna do that at my Work.

When you insert the part containing sketch into your new part, in the first dialouge box which actually comes up in feature tree, you have to select unabsorbed sketch & absorbed sketch(in case of extrude)Select both to be on safe side.

But I think you should try the sketch in a assembly & then create parts in the same assembly, that will save you time in assembling them later. & it will update faster than the insert part method.

Hope that helps.

 

[KirbyWan]

Arrrrgggghhhh.

How did I miss that option. I looked down that list and no light bulb went on. Mea Culpa. (<-- That's latin for me slapping my forhead.)

-Kirby

Kirby Wilkerson

Remember, first define the problem, then solve it.

 

[KirbyWan]

O.K. I got this to work, but with a (minor) problem. I have created each part based on a single sketch. I then create an assembly with all the parts using the tooling holes as the mates. If I then change the dimension on a tooling hole, it breaks all the mates between the tooling holes. I can live with it because I'm just using the assembly to check that everything looks right, but I feel it should not break the mates.

Is there a best practice to avoid this? for example pick mates that are not going to change dimensions? The tooling holes need to match a bond tool, so I get a first article set of sheet metal parts and put them on the bond tool and measure how far off I was and then update the parts (once hopefully.)

Thanks for everyones help. I feel I really learned something.

-Kirby

Kirby Wilkerson

Remember, first define the problem, then solve it.