Inventor 2016 Large Dimension Shrinkwrap Assembly To Part Cannot Cut/Split Solid

[Jose_Merino]

Good Evening, I use Inventor 2016, I have this building (fig 1), I make this building a simple part to make the modifications more easy, I need to cut this building, I need sections of it no complete, but I tried a lot of thing and nothings works, I try to make a cut with the extrusion command, I try to make a split, and same thing I tried with view and make a half section view, this work, but I can't make another half section view in the other end of the building, because my first half section view disappears and all my building is complete again, any body have an idea how i cut this building in sections?

Thank You.

Fig. 1

  kelly.young has edited your subject line for clarity: Cut a Piece

[johnsonshiue]

Hi! How big is the structure. Is it within +-100m in X, Y, and Z? And, is the length of any geometry less than 100m?

Many thanks!

[Jose_Merino]

My building is X=250 m, Y=75 m and Z=25 m, the pieces that I want to cut are less than 100 m, for example I want o make a cut just for the column 4 and 3, wich is only 8 m.

Thank You.

[johnsonshiue]

Hi Jose,

Without seeing the actual file, it is hard to say. But, I don't think it will work. Although the geometry you are trying to operate is within the model range. The part consists only one body. When the cut happens, the entire body needs to participate in the operation. X=250m is too big for Inventor unfortunately. Do you have to include everything in this part? It looks like a derived assembly. Could you exclude certain sections?

Many thanks!

[subhashmecha]

Hi Jose, 

I can see that you made the building assembly file as a part file. Why don't we use split command and split into 2 bodies and isolate the part you want. 

attached link of how to use split command:

https://designandmotion.net/autodesk/inventor-using-split-solid/ 

Let me know if it's work out.

[Jose_Merino]

I try do the split, but it take a long time and after all it told me that he can't do the split.

[swalton]

@johnsonshiue is referring to the maximum component size in a part file.  It is limited to 100m (see my question below) in any direction.  Inventor's behavior with parts that exceed the limit is unpredictable.  Any given command may or may not work.

You will need to trim down your assembly before you do your shrinkwrap.  Use an assembly cut (or a LOD or maybe a Design View Rep) to get rid of the building length that you don't need, make your shrinkwrap, suppress the link in the derived part, then suppress the cut in the parent assembly.  Repeat the process whenever you need to push changes from the assembly into the shirnkwrap.

Johnson, the knowledge base article linked below suggests that the limit is a 100 meter cube, centered on the origin.  I take that to mean +-50 meters along any axis.  I read your statement as that the limit is +-100 meters along any axis.  Which is correct? Could a dimensioned drawing/picture be added to this article to help explain?  I think Autodesk might have some software that would help making that picture.

See: https://knowledge.autodesk.com/support/inventor-products/learn-explore/caas/sfdcarticles/sfdcarticle...

[johnsonshiue]

Hi Steve,

The article you cited is a bit confusing. Here is the updated version. That old article should have been removed. This is about floating point numbers handling. So, the geometry has to be located within +-100m in X, Y, and Z (not a cube of 100mx100mx100m centered at origin). And, the actual size of each geometry has to be smaller than 100m.

https://knowledge.autodesk.com/search-result/caas/CloudHelp/cloudhelp/2017/ENU/Inventor-Help/files/G...

Many thanks!

[swalton]

Johnson,

Thanks for the update.  

The confusing article was one of the first that came up with a "bing" search.