NX - Body not able to divide into two pieces 1

[sunnylooks]

thread561-195944
I have a iges model (Hollow from inside) which i want to cut into 2 equal pieces
But i have tried:
Split
Divide
Trim body
Extracting and then sew all the faces
But still every time it says bodies create into multiple bodies.

I am using NX7.5
I have attached the model for your reference -

http://files.engineering.com/getfil...-df6576a168a5&file=93241951_Two_cyl_Block.igs

Please help me ASAP

 

[wackolacko]

Here you go.

John Lackowski
NX Support
Win 7 64bit NX 7.5.4.4 TC 8.3.1.1

 

[wackolacko]

Or this one...thickness maintained.

John Lackowski
NX Support
Win 7 64bit NX 7.5.4.4 TC 8.3.1.1

 

[mmauldin]

I couldn't get anything to work until I exported the file as a STEP file, then opened the Step directly. Lot of weird stuff happened with the original file such as subtracts being performed as unites.

Attached is the split body file

 

[Toost]

This is one of the very rare cases where the solid body is "inside out". On a normal/valid solid body, all face normals point out, away from the volume. On this one all(*) point inwards. If you use for example the Synchronous Optimize face feature, NX will reverse the normals into a valid body.
Probably also functions such as File - Export -Heal geometry will repair the part.

Just for fun, try placing a view of the model on a drawing and see how strange the result becomes.

* Use Information -Object and select some face-s, the arrow displayed should point out, not in.
( I did not check all faces, maybe 10 .)


Regards,
Tomas

 

[sunnylooks]

Thanks everybody for very quick response but none of the file attached is not opening in my UG.
Also i have 3 other parts to be completed so please let me know how to create split onto it.
Please list down some steps for how to do

 

[mmauldin]

The file I submitted is NX7.5, don't know why it won't open.

To fix your file go to Insert> Synchronous Modeling> Optimize> Optimize Face, then select all of the body faces and and hit "OK". You should be able to split the body using the normal split command.

If that doesn't work, export the parts as STEP files (File> Export> STEP203) and either re-import them or open the STEP directly using File> Open and selecting the *.stp file type option.

 

[sunnylooks]

mmauldin thanks for the details advice...
Actually today i am using NX6 workstation n not NX 7.5.
Is Optimize face command available in NX6????

exporting to .step and importing is not working....i tried it same problem....i even tried exporting to .parasolid n importing but same problem.

Please suggest

 

[mmauldin]

I don't seem to remember Synchronous modeling being available in NX6.

Try File>Export>Heal Geometry as Toost noted earlier. It works to fix the file in NX7.5.

Attached is the STEP file I used.

 

[cowski]

Synchronous is in NX6, but not "optimize face"...

www.nxjournaling.com

 

[wackolacko]

ok, here is a NX6 Parasolid for you.

John Lackowski
NX Support
Win 7 64bit NX 7.5.4.4 TC 8.3.1.1

 

[sunnylooks]

Dear John,
Thanks for your help and paras solid model.I have got 3 more other models to do the same.

I want to know how it can be done in NX6.so that i could apply it in other 3 also.

 

[Toost]

Sunnylooks,
if you read the thread above, you will notice that I have proposed the Heal Geometry option and that Mmauldin has commented on this and noted that the Heal Geometry works. I have now myself tried the Heal Geometry , in NX6, and again noted that it works.
Other users has reported that doing a Step Export -Import also repairs this model.

Is there anything more to say ?

Regards,
Tomas

 

[sunnylooks]

Thomas your are perfectly right...but both the options are not working at my end...

 

[wackolacko]

All I did was File -> Export -> Heal Part

John Lackowski
NX Support
Win 7 64bit NX 7.5.4.4 TC 8.3.1.1

 

[Toost]

Sunnylooks,
When you use the heal geometry option, are you aware that NX will create a new partfile containing the "healed" body ?
The one you "exported from" will not be changed in any way, you have to open the healed partfile and use that instead.

Regards,
Tomas