difficulties with dimensions in 2d drawing of solid imported as step file

[Anonymous]

Hi,

I am totally new to Inventor 2020. I apologise in advance if the question is banal.

I imported a STEP file and created a drawing of it. I need to show the dimensions in each projection, but I cannot retrieve them. If I select an edge, whose dimension I want to show, the dimension does not even appear.

Thanks in advance

Alessandro

[jhackney1972]

I have included a quick demo Screencast of taking a STEP file into Inventor 2020 and then to a drawing view.  Then I drop a few dimensions on it.  The only thing I can think of that may be giving you trouble is your STEP is corrupt.  Please attach it to your forum post so the forum users can troubleshoot it for you.  If you do not know how to attach it, Zip up the STEP file and then attach it using the Attachment section of a forum post.

[Anonymous]

Hi John,

Thanks for replying so soon.

When I try to select an edge to get its length, it becomes red instead of green, so I guess it indicates some kind of error.

I have attached the STEP file now.

Thanks

[jhackney1972]

Sorry for the delay.  Your step file is giving me some difficulties creating dimensions in the 2D drawing.  Some views work fine and other views will not dimension correctly at all.  The Screencast will show my difficulty.  I hope someone else has a cure for this.

[Anonymous]

Thanks a lot!

[jrobrador19 · Accepted solution]

Hi there,

Like @jhackney1972 I'm also having a difficulty placing the dimensions for some reason. If you really need those dimensions in your drawing file, what you can do is to create a sketch overlapping the view in the drawing creation environment. So basically, the sketch is getting dimensioned instead of the 3d model.

Object snaps are still present and should be able to help you draw your lines and arcs. There's no need to sketch everything, just sketch whatever you need to dimension. This is not totally a solution but just a workaround to help you in some way.

I hope this helps.

[JDMather]

I would use only as reference in remodeling from scratch.

What software did this STEP file come from?

In Shaded with Edges visual style, note that there are no boundary edges for the "fillets".

[SBix26]

This is a very odd STEP file.  Can you tell us more about its origin?  The perimeters of both solid bodies are single surfaces, and the translation report gives the same warning twice: "Some Surfaces have been simplified".  These single-surface perimeters don't allow measurements, so I suspect that they are actually spline surfaces.  You can get most of the dimensions by placing projected drawing views, but the corner radii require projecting them into a sketch (drawing or model) and constraining arcs over them (turns out they are 2mm and 19mm respectively).

The translation report says that the sending system was "HarmonyWare Translators"

With these particular solid bodies, they appear to be nothing more than rectangular plates with corner fillets.  I recommend that you re-create them in Inventor.

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Sam B
Inventor Pro 2021.1.1 | Windows 10 Home 2004
LinkedIn

[Anonymous]

Thanks to all for your help.

I guess the solution here is only the workaround of overlapping a sketch onto my objects. 

The origin of the STEP file is CAESES, a piece of software developed by FRIENDSHIP (https://www.caeses.com/), which works pretty well for parametric ship design, or parametric design in general. The flat plate in this example was just my basis, I had to build some particular shapes on top of it.

Usually the STEP/IGES files I generate work fine when I import them into CFD programmes, so I hoped I could do the same with Inventor.

Thank you very much again for your help

[johnsonshiue]

Hi! The STEP file was generated by "HarmonyWare Translators." I have to say this is the first time I heard about the vendor. Except the planar faces at top and the bottom, the side faces are all spline. This is why the geometry cannot be dimensioned easily, though it looks straight. If I were you, I would simply completely recreate it in Inventor using proper sketch and extrude. Then the drawing view will be precise.

This is another example of manipulating imprecise data on a precise modeler. It is not an ideal workflow. Likely the result will not be desirable.

Many thanks!