Master sketch modeling

Hello all,

I start with Skeleton modeling in Inventor 2015 and I would like to ask you for couple of advice or clarifications:

1) In case I make a master sketch (.ipt) for big assembly, how should I organize the browser where I have lot of sketches, work planes and surfaces....can I make some root system there.....e.g. sub-master sketches in the master sketch browser?

It looks like very chaotic if I put all these working features in same level.

2) Is there a way how can I put once made master sketch for a part into the assembly master sketch which I am going to do?

For example: I have a parametric master skecth for Part X as well as for Part Y and these I would like to use in the parametric master sketch for the Assembly XY.

3) In case I have same parts (sketches) in the master sketch...should I make sketch in the master sketch for each part?

Thank you for your help, Vlada

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4 Answers

There are a few options for "skeleton" modelling:

.ipt with sketches only (let's say you build a mechanism):
In the sketch you group the lines in blocks and rename the blocks to make more sense. This is where you can test the mechanism by dragging the levers. You can add new sketches (on same/different planes) and project points/lines as needed. Now you "make components" – select the sketches. An assembly will be created with the parts named as per the blocks, placed as per the sketch(es). No constrains added. Each part will have the dedicated block (same name) and sketch embedded in it. This is linked to the original sketch: Original sketch is the “parent”. Change the sketch and the components change.

So, to answer your question 1)… group the lines in block and rename them. Separate sketches for the sub-assemblies – but will create ONE assembly with all of the part in. You will have to demote the parts into sub-assemblies… and constrain them.

Question 2)… the sketches (containing the blocks) will be in the parts when you “make components” Part X will be made from BlockX.

Question 3)… sort of: the blocks will make the parts / sub-assemblies. Can be one sketch. Can be more.

Note that you can have blocks within blocks. This block will make a subassembly in the new assembly when you “make components”.

Another option would be: Build a part (.ipt) with multiple solids:
Model the whole assembly as a single part with separate solids. Rename the solids to make sense. “Make components” – select the solids individually. An assembly will be created with the parts named as per the solids, placed and GROUNDED as in the original part. No other constraints added. (You will have to demote the parts into sub-assemblies). The main advantage here is that you can project edges in the part without creating external “adaptive” features.You can rework (add features to) the new components, but the original part will drive changes down to these components (where you may lose the reworked features). These components are linked to the original part: Original part is the “parent”. Change the original part, and the components change after you update them.

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Thank you for your article. I tried the first option but I got stucked on the part which needs lines in different sketches and different work planes.
Is the first option usable in case I have a part which is made of several different sketches in different planes?
I added some pictures from my trial design.
I made a parametric ref.sketch for a tank contains a steel frame and a plastic tank. It would be ok, if I finish my effort only with this tank. Number of planes, sketches and splits is not so huge to be chaotic. But anyway, I would like to order items in the browser for the steel frame and for the plastic tank. But sketches for both are not in same plane.

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My pleasure :-)

I think you over-complicated that model a bit. I use basically the same setup as the one I did for this tank (didn't do the bottom frame - oops) for when I build big structural buildings... I added the pack-and-go for the tank in the 7zip file

For your tank: The part file that will become the skeleton for the frame-gen assy may have solids in = the plastic tank itself. then I draw sketches on the faces and project the points/lines to the other faces so they line up. The split features in your sketch could be replaced with workplane-sketch-project cut edges to give you the sketchlines for that level.

For a big structural building: I build the concrete foundation - then on the top I add the sketch for the bases - then offset workplane... new sketch... project points... draw lines... - then offset from bases next workplane... new sketch... project points from bases... draw lines... etc. The same idea: base/skeleton sketch part will have solid in for concrete foundation. The sketches in this base/skeleton part will drive the frame-gen for the columns / beams.

The process I described in my previous answer is more for mechanical setups where you build the assembly using the base part to drive the form.

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Sorry for not answering yet, but I still try your way to implement it for my exact case to make it the most functionable.
I come back soon.

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