Top Down Design fo Beginner

[nige106]

Hi,

I've recently started using Inventor and my background has always been AutoCAD based. I'm starting to try to create more complex frames. I'd like to plan the frame in 2D then create parts/features from this. I know I can use the frame design tool but there are some designs I'm struggling for it to work with.

So heres my flow so far:

I create the sketch in 2D within a part file.

I then add this into an assembly to act as my template

Now whenever I try to create new part files for the various pieces I can project geometry but if I amend the original sketch nothing updates.

I may not have explained this very well and maybe there is a better way for me to do this? I basically want the part files to update in length/size/feature position when the original sketch is modified.

Help.

[JDMather]

You should not have to project geometry (not sure what that means in the context of what you are doing, unless this is for mounting holes or something similar).

Attach your files here.

[ampster401]

research "Skeleton Modeling" or "Master sketch modeling"...

http://www.kwikmcad.com/iclips/imaster.aspx

HTH

[nige106]

I've hopefully linked some test files I've been playing with over Lunch. I create a skecth then used derived component to create the part.

http://totalsolutions.livedrive.com/item/6b21b4de1749403da738b6a477b6930c

[nige106]

Thanks for the link, I'm downloading it now.

[JDMather]

Attach, not link. 
Attach your files here.

[nige106]

Part files attcahed to this post

[nige106]

Assembly attached to this post.

[nige106]

This is the AutoCAD version of what I'm trying to create:

[Curtis_Waguespack]

Hi nige106,

One general tip that might help is to know that you needn't have sketches to use the FG  (Frame Generator). Instead you can create a solid that defines the shape of your frame and use the edges to place frame members. FG automatically projects the geometry into the skeleton file that it creates using the selected edges.

For instance if you were trying to create this frame:

 

You could just create a solid like this:

 

If you need more edges you can sketch on the faces of the solid:

Using this method creates a more robust skeleton and is generally very quick to create and update.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[nige106]

Thanks for the info Curtis. I've been playing with the frame generator and 95% of the time I think it shall be all I need.

I may have partly managed to do what I wanted, by creating a master part file with all my sketch geometry in then creating part files as derived components referencing the master part file.

I've attached my files as a zip file. Test.iam is the completed assembly. Test1.ipt is the master sketch geometry. The other 4 files are the components.

Anything anyone would change?

[nige106]

Okay, I've managed to create my master sketch and when I update parameters everything changes as I want.

Now when I model the part files is it best to have a single tube in each part file or is it okay to use multi bodies and have several tubes in the same part file?

[nige106]

Okay, on smaller projects I've started to try and use inventor to create the models.

My workflow is:

Create initial sketches in a part file (master.ipt)

 

I then extrude each individual shape that shall become a componment into a solid

 

I use "make parts" and send the solids as surfaces out to assembly and part files. In this case I did this twice as there were only two components and ended up with truss block.ipt, truss block.iam and corner block.ipt, corner block.iam.

I also use "make part" to create a derived part file with just the sketches in (sketch.ipt)

I then create an assembly (Overall.iam) insert all the assembly files and the sketch part file and constrain as required

I now go into the part files (truss block.ipt) and start to flesh out member positions using sketches. I create multiple bodies in one file. I then use make components to split all the solid bodies out to individual part files but within the original assembly (truss block.iam). I then constrain all the parts correctly.

Now when I go back to the Overall.iam I can remove the visibilty of the derived surface to just leave the solid parts

I can now edit the original sketches in master.ipt and the Overall.iam updates.

Does anyone have an easier method of skeletal/top down modeling? I'm still new to modeling this way so any help shall be appreciated. I want to try and get my work flow correct before attempting anyhting larger and ending up in a mess.

Now the reasons I like this method is that I can quickly create lots of solids in the original sketch and get a feel for how the whole design shall tie together without worrying about details at this early design stage. I sometimes struggle to work with 2d sketches on complex designs so seeing a 3d item is easier. The final assembly also doesn't contain the original solids so the weight calculations aren't thrown out.

Files are attached

[nige106]

More files

[nige106]

more files

[nige106]

more files

[JDMather]

I'm not sure I followed everything (didn't open the files), but you can extrude surfaces directly - you don't need to create derived part.

[nige106]

This is more typical of the type of design I'm creating where I just want to flesh out the shape to then return and fill in details such as connections and member sizes. There'd be 13 different assemblies to create the complete grid.

[nige106]

So rather than extruding solids in the original master.ipt extrude surfaces? Is it best to patch the open ends so I can sketch on them easily in the future? Once I have this geometry to work from would you then still use "make part"? I can't select the surfaces if I try to use "make components".

I liked extruding to solids as it's easy to work on the model by having non transparent faces.

[JDMather]

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@nige106 wrote:

I liked extruding to solids as it's easy to work on the model by having non transparent faces.

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I didn't fully check out what you are doing.  Sounds like you have it figured out.
I was going to suggest another workflow with Extruded Solids but set to Water or Polycarbonate for visibility through the skeleton, but it sounds like that isn't what you were after.