Scaling an assembly

[Yashasvi23481]

Hi All,

    I am using Inventor 2018. I have a peculiar situation. Not sure if it has been covered before or possible at all.

       I am after a 3d model, from which I have to create a skeleton model using silhouettes (2D side plates from front view and side views). I manage to get free version from online but its scale is 1:13.5 when measured and compared with actual size. For example, Width on actual model is 3.6m but model I downloaded from inventor was 206mm which is 13.5 times smaller. I have downloaded as individual parts from step file conversion screen assuming it will be 1: 1. 

Instead of going through scaling individual components to 13.5 to meet actual dimensions, I was wondering if I can scale whole assembly. Is that possible ? All components are grounded and when I ungrounded, all are floating in air with no constraints. there are 15 to 20 individual parts and I don't want to waste time as I need only for creating prototype model But side and rear panels will need to be correct. Is it possible in Inventor to scale it (assembly) or I convert to AutoCAD prepare silhouttes (panels) and extrude in Inventor and re assemble ?

See attached pdf of what I am trying to achieve. from actual model I created a prototype of 4 walls taking outline. 

    I can think of 2 options: 

1. create views in inventor drawing using existing scale, export to AutoCAD and rescale each view to desired size and then extrude using ipt again in inventor.

2. Download the step file using composite instead of individual which is like envelop and then rescale in parameters applying 13.5* each value and then create 2D drawings in Inventor. 

 Is there any alternative option / solution ? 

[SBix26 · Accepted solution]

Scaling of each of twenty components using Direct Edit tool would be much quicker than the proposed AutoCAD method, in my estimation.  Open the component, click the Direct Edit tool, change method to Scale, select the solid body, relocate the triad to the part origin, OK.

---

Sam B
Inventor Pro 2019.2 | Windows 7 SP1
LinkedIn

[WHolzwarth · Accepted solution]

I'd try this way:

- Import STEP into Inventor the normal way. Perhaps it comes in as IAM, perhaps as multibody (MBP); doesn't matter.

- Save that geometries

- Open new IPT

- Ribbon Create ->Derive. Open the above IAM or IPT.

- In Derived part window, set Derive style to 3rd option. There you can apply a Scale factor. Result will be a MBP in new size.

- Make components of MBP members after that.

[johnsonshiue · Accepted solution]

Hi! Similar to Walter's suggestion, there is a way to do it through neutral format like SAT. You can simply export the assembly as a SAT file. Then edit the SAT file in Notepad. The third line in the file starts with the scale factor. The default is 1. You can change it to anything you like. Then import the SAT file to a desirable unit. The imported geometry will be scaled.

Many thanks!

[Yashasvi23481]

Hi Sam, Walter and Johnson,

    Thank you so much for the resolution. Will do so. Really helped. Tried all three. 

Kind Regards,

Yash