It sounds like your colleague is looking for a model with the parametric history that created the part. When he says "flat" he might be referring to the the lack of the parametric relations. And he can't "edit" the part if there is no parametric history.
Unfortunately you won't be able to give him a parametric model from Rhino if that is what he wants. You should could clarify this with him.
FYI, Parametric construction history is specific to the application, and common file formats like STEP, IGES, ASIS do not contain that history. So in general, if someone wants a parametric model in SolidWorks, it has to be built in SolidWorks.
It has been 5 years since I worked with Rhino files so this could be wrong but, As I recall I imported the Rhino files in STP or IGES and they came in as surfaces. I then had to learn and use surfacing to create new surfaces, create parting lines for separate parts, and then thicken the surfaces into solids. Not much fun when you have never worked with surfaces but it will give him a chance to broaden his skills.
Also be sure to coordinate weather they thicken in or out as this can make a big difference.
I have Rhino version 3, so I am not sure what all is different in Rhino version 5. I have also never used Rhino to make drawings. But no matter what, exported "drawings" from Rhino will never be able to be edited in Solidworks. Exported models from Rhino will come in as an imported solid in Solidworks (providing it was properly modeled up in Rhino).
Can you upload one of the files you are attempting to send, that the other person is having problems with?
One other thing that needs to be clarified...
I get the impression that you (or maybe the person in China) might be using the words "drawings" and "models" interchangeably. If that is the case, please understand that they are not interchangeable terms/words. There may be a communication disconnect happening here.
Sorry for the miscommunication. What I ment by "drawings" are 3D Rhinoceros models which I have converted into IGES, STEP and ACIS.
Does running FeatureWorks help recognizing the features when they load in the Rhino models?
This really depends on the complexity of your model. It does not work boundary surfaces, or fillets adjoining those surfaces. So if your model has organic or freeform surfaces, it may not help very much.
Here's the list of what it can do from the Help/Knowledge Base:
The FeatureWorks software recognizes features on an imported solid body in a SolidWorks part document.
Recognized features are the same as features that you create using the SolidWorks software. You can edit the definition of recognized features to change their parameters. For features that are based on sketches, after you recognize the features, you can edit the sketches from the SolidWorks FeatureManager design tree to change the geometry of the features.
FeatureWorks recognizes the following features:
- Extruded or revolved features
- Chamfers on linear or circular edges
- Constant or variable radius fillets on linear or circular edges
- Ribs: extruded parallel to sketch, extruded normal to sketch, and ribs with negative draft.
- Draft features
- Holes. With automatic or interactive feature recognition, you can recognize these types of holes: simple, simple drilled, taper, taper drilled, countersunk, countersunk drilled, counter bored, counter bored drilled, counter drilled, and counter drilled drilled. You can also recognize Hole Wizard holes.
- Lofts. Interactively recognize base-lofts.
- Sweeps. Interactively recognize boss and cut sweeps.
- Volume Features
- Feature patterns: linear, circular, rectangular, and mirror.
- Sheet metal features: base flanges, edge flanges, sketched bends, hem flanges, and miter flanges.
- Sketch Patterns. Using interactive recognition, you can create a sketch pattern from similar features that were created randomly. Partial imprints of features cannot be recognized. Creating a pattern of a pattern feature is not supported.
- Multibody parts. Recognize Multimode parts one body at a time.
FeatureWorks can automatically add dimensions to features it recognizes. It supports baseline, change, and ordinate dimensioning schemes and recognizes concentric and other relations. See Recognized Sketch Constraints for more information.
I have never found Featureworks to be all that useful...unless the model is exceptionally simple (in which case I get a better feature tree by simply creating the model from scratch).
IGES, STEP, ACIS, and any/all other type of "neutral" file formats do not contain "how it was built" data...they only contain a definition of the model as it existed at the moment you created the file. No "history", no "feature tree", nothing along those lines. And unless Rhino has changed significantly since version 3, Rhino itself has no feature tree. So even if Solidworks could read in the native Rhino file there would be no feature tree to it, and that is the only way Solidworks would be able to read in a file created in another system and bring it in with a complete feature tree. If I make an IGES, STEP, ACIS, Parasolid, or some other type of "neutral" file type of a model I created in Solidworks...it will not come in as a model with a feature tree. Those file formats are not able to convey that information. And Rhino doesn't even have it to give, even if they could. Those file types are like a polaroid photograph...tap the photograph all you want, it won't play a video.
If possible, please upload one of the files you have sent out, that is coming in to Solidworks "flat".
I can pull it into Rhino and Solidworks and might be able to help you.
(Solidworks sometimes tries too hard to be "smart" when importing things...and ends up making some bad assumptions. Rhino, on the other hand, makes no assumptions when importing a file. It just pulls it all in.)