Change imported assembly from inch to mm

[Anonymous]

Hello,

I am new to inventor and am having trouble converting an imported creo assembly from inch to mm. Is there a way to convert 1 inch to 1 mm?

[johnsonshiue]

Hi! I think this is indeed about rescaling the entire assembly. Please take a look at post #20 and follow the instruction. You can export the assembly as STEP and change the scale setting. Or, open each part and use Direct Edit -> Bodies -> Scale.

Many thanks!

[Anonymous]

Hello Johnson, can you please send a link to this post. Thank you

[WHolzwarth]

Meanwhile I tried several ways of solving this problem, but with no pleasure.

Similar as Johnson I thought of exporting as STEP, changing units with an editor, and saving back as STEP. I've found this line: 73266 CONVERSION_BASED_UNIT('inch',#70334) , but courage left me with changing.

Another attempt was opening the STEP in Rhino6, scaling it down with factor 25.4, and re-importing that. But result was only a multibody with no sub-assembly structures.

I didn't try scaling down of each IPT with factor 25.4, because it's a whole bunch of work. And I think, that part placement in sub-assys is damaged after that.

And I've tried setting up import units with an Inventor version earlier than the AnyCAD era, but I always got the same result. Import took some time, and I expected  a faster result.

Conclusion: A scaling option for a top-level assembly and all it's members could have helped here. But I didn't find the way to go.

Right now seems to be the best way saving a derived component, making parts, and re-placing them back in sub-assys.

But I'm only a single forum reader among many others. Perhaps there's a much better road to Rome with access to the initial Creo file..

[johnsonshiue · Accepted solution]

Hi Guys,

I think I have found a solution. The workaround I mentioned above still works but the original Inventor files will need to be modified. The issue with this dataset is that the components were modeled in mixed units. Some are in inch and some are in "mm." To ensure true dimensions, Inventor converts all length values to mm in STEP so that there is no ambiguity. The length values in the STEP from the original file are all in mm (you see values like 254).

What I did was pretty simple but a bit tedious. I just open each Inventor file and change the unit to inch. Then export the entire assembly as STEP. The length values in the STEP file will be in inch. Lastly, I change the scale factor in the STEP as discussed earlier. Now, the STEP file imports as mm (see attached files).

Many thanks!

[Anonymous]

Hello Johnson, thank you for your solution, much appreciated. I took your earlier advice and opened every file, converted to mm and re-constrained. thank you to all who helped solve this issue

[Anonymous]

Actually IV should work in mm from start and not convert to mm on export ("to avoid ambiguity"). If you only have one internal unit then you can mix files in whatever visible units without touching the true dimensions. This is an autocad heritage where you only have numbers inside and you can decide from the outside what these numbers represent, millimeters, inches, miles or lightyears...

US is the last country, besides Liberia and Myanmar, to have inches as standard unit.

And inches are everywhere in the guts of IV. I recognise the tracks (2,54mm text size...) from a mile away (pun intended).

[johnsonshiue]

Hi Alex,

Let me clarify a little bit. Inventor does have an internal unit (cm). This is why Inventor supports mixed unit modeling, i.e. inch parts can co-exist with mm parts without a problem. This is the bread-and-butter workflow from day 1.

The geometry created in Inventor and its competitors like Creo and SWX is always true length. It does not matter what unit you choose per part. The length is absolute regardless of units.

What the OP was asking is unorthodox to true length modelers. He is asking Inventor to change global scale for all components within the assembly. The original design was in inch incorrectly as opposed to desirable mm. The solution I proposed to him is a hack actually. Essentially, I tweak the STEP file and trick Inventor to rescale the geometry. This is not a normal process. The alternative is to recreate the part to the right scale or use Direct Edit to scale the model individually.

The need to unify the unit in this case is to homogenize the STEP data into values in inches. Otherwise, they will all be converted to mm in STEP due to the mix-unit geometry and the rescaling would not happen. This hack allows the geometry to start with values in inches but end up with scaled down model in mm.

Many thanks!

[Frederick_Law]

Johnson:

Not related to OP's problem.

I think when exporting assembly in Inventor with parts modeled in mm and inch, the STEP file will have wrong scale.

[WHolzwarth]

I could think of an iLogic or VBA routine, that's scaling a whole assembly and it's members with only a single mouse-click.

But I didn't find anything like that.

[johnsonshiue]

 Hi Fredrick,

I am sorry I don't follow you. Inventor supports mixed unit modeling. The components can be modeled in any supported unit with true scale and true length. It does not matter what unit is used. An assembly can contain parts in various units. STEP export will still be correct. Could you share an example of out-of-scale behavior?

Many thanks!

[Frederick_Law]

Don't have an example.  I'll try to create one.

Here is a description.

Inventor part and assembly can be mm or inch, setting in document option.

If assembly is mm, two parts are added to the assembly.

One is mm, one is inch.

Export assembly to STEP.

Reimport STEP into Inventor and one of the part will be wrong scale.

If I remember correctly, import the STEP in other software will have same result.

We notice that when using customer files and other 3rd party (McMaster, Parker, Misumi) files in same assembly.

Solution was change all ipt and iam to same unit before export.

That was on IV2012.

[johnsonshiue]

Hi Frederick,

It might be the case in the past 2012 or earlier. It was a bug. But, from 2013 and later, I don't think that is the behavior. It should work always work regardless of units. If you have an example showing it otherwise, please let me know asap ([email protected]).

Many thanks!