My goal is to create an air-solid model for a turbomachinery blade passage to be used for unstrcutured meshing in NX.
I have 6 surfaces now (inlet/outlet, hub/casing, periodic up/down). I sew them together to form an air-solid body by Menu --> Insert --> Combine --> Sew, Type = Sheet, Tolerance = 0.0004 (Default) (Fig.1)
The next step would be to trim this air-solid body by a 3D blade surface that extends beyond the hub and casing faces to add an internal blade surface. I do this by Menu --> Insert --> Trim --> Trim Body (Fig. 2) The problem can already be seen in Fig.2:The sewn body is NOT air solid as I expected. It is merely 6 surfaces joined together. Therefore when I trim this sewn "body", only the hub and casing surfaces are to be trimmed (you could see that only the hub and casing airfoil profiles are highlighted in Fig. 2, otherwise the whole 3D blade should be highlighted). Fig. 3 is after I click on "Reverse Direction" to complete the trim.
What did I do wrong? How can I address this issue? How to make sure the Sew process generates an air-solid body? Any idea would be appreciated. Thank you very much!
Solved! Go to Solution.
Assuming that you your Body Type Modeling Preference is set to Solid Body, my guess is that you have gaps between your surfaces that are larger than your 0.0004 Sew Tolerance and hence creating a sheet body rather than a solid body. Having selected your Target and Tool surfaces, use Show Result to see if any asterisks are displayed along the edges of your surfaces - that would indicate gaps larger than the tolerance. Then either review/correct your surfaces to reduce the gaps, or adjust your tolerance to accomodate the gaps.
Thank you for your reply! You made me realize that my problem lies in me having Body Type Modeling Preference set to Sheet Body, not Solid Body... Now that I used the correct Body Type setting, I am able to get an air-solid body after performing the Sew command.
However, I am having problem with the next step i.e. Trim Body. When using the 3D blade surface (i.e. Sew(163) in red) as the Tool to trim the Target the air-solid body (in light blue), I'm getting an error "The tool and target do not form a complete intersection". I adjusted the tolerance up to 1 [in] but the error persisted.
To me there is a complete intersection, so something must be wrong that I'm not aware of. Perhaps telling you a little bit about how the 3D blade sheet body is generated may be helpful for diagnosis. The 3D blade surface is 3 pieces sewn together. The upper and lower portions are splitted bodies out of one sheet body. The middle portion is a sheet body generated from a solid body using the 3rd approach you suggested in this post.
Can you give me any ideas or suggestions to resolve the issue? Thank you!
Just an idea to check the complete intersection issue..
Give some thickness (1mm..) to the sheet body (in the direction of the to-be removed trimmed portion) and then do an intersection (boolean) of the two bodies (the thickened body and the main solid lade body on which you are trying the trim operation.)...do you get any intersect body?
Hi @kapilsharma - Thank you for your time and reply. I have to admit I don't know how to do what you suggested in NX, so I didn't try it. Hopefully it may inspire other people who run into similar problem.
Hi @@BenBroad - Since you mentioned tolerance and asterisks, I repeated the process of sewing together a 3D blade paying particular attention to avoid asterisks. This time, using this blade sheet body, I am able to trim the sair-solid body without getting any error, thanks to you.
Sorry i should have elaborated on it better. But now it is hardly needed as Ben has already solved it