Creating solid from surfaces 1

[MichaelkSA]

I know that if you 'sew' different surfaces together and if they form a water-tight body, the resulting 'sew' should be a solid.

The problem is, even though the surfaces I sew together seem to form a water-tight body the result I get is still a sheet body and not a solid, no matter how high I make the tolerance.

is there a function to test the water-tightness of a body?

I will really appreciate it if someone can give me a hand. The part file is attached.

Michael

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[Toost]

The tool I use is Examine Geometry, it has a special check for Sheet boundaries, After checking, you can tick a checkbox and NX will highlight the open edges. ( Which you then when you know where it's at can check for the deviation etc.)
Also, if you press Apply in the "sew" dialog, NX will highlight the open edges. ( Pressing OK does not.)

Screenshot from Examine Geometry.

Regards,
Tomas

 

[MichaelkSA]

Thank you Tom. That was exactly the function I was looking for!

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[Xwheelguy]

First thing I'd check is Preferences -> Modeling and make sure Body Type is set to Solid.

Tim Flater
NX Designer
NX 9.0.2.5 Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB

 

[JohnRBaker]

When you say that "no matter how high I make the tolerance" please explain exactly what you mean. Are we talking INCREASING or DECREASING the value of the 'Distance' tolerance? Making the value SMALLER, or DECREASING, the 'Distance' tolerance will NOT help you get a better result. In fact it will prevent you from getting what you want. If you have problem sewing sheet bodies together, you should INCREASE that it make LARGER the value of the tolerance. Now there is a point where increasing the value will become a problem but for now try moving it that direction firat.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[MichaelkSA]

John,

I did indeed increase the value of the distance tolerance. I even increased it to a ridiculous large value and it would still not stitch it to a solid.

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[JohnRBaker]

Then you've probably gotten some really bad data or the gaps are so large that NX can't 'heal' what are basically 'gaps' in your original data.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[cowski]

Also note that if you sew all the sheets together and it results in a sheet body (due to gaps), no future edits to that sew feature will result in a solid body (i.e. changing the tolerance after creating the sew feature will not result in a solid body being created). With sew: once a sheet body, always a sheet body. If you were expecting a solid body to result (which it will if there are no gaps) but get a sheet body, look for sheet boundaries (as outlined by Toost). Delete the sew feature, edit the sheets as necessary and try again. If deleting the sew feature would result in a loss of other features, you could try a work-around. Make the sew feature current and edit it to remove one or more sheets; then create a new sew feature to add them back in (make sure to check that the result is a solid).

 

[jerry1423]

Is it possible to post a parasolid of these sheet bodies ?
I am on NX7.5, which is older than the part file was posted.

Jerry J.
Milwaukee Electric Tool

http://www.milwaukeetool.com/

 

[Drew4792]

Do you have duplicate surfaces? I have had surfaces on top of a surface. If this is the case it will not become a solid.

 

[Xwheelguy]

He's attached the model beneath his signature - not sure what version of NX he's using, but it opens in NX9 for me.

For starters, the base surfaces are not up to par - they "look" fine, but aren't G1 or G2 and 3 sided surfaces are used intermittently. Those issues may compound with the Patch Openings that are being used downstream. The base surfaces need to be extracted, untrimmed or Delete Edge used and recreated with a minimum of G1 where applicable. The cockpit area will get messy because the untrimmed edges won't line up.

Prime example where the underlying curve network was not up to par, therefore the resulting surfaces wouldn't Sew together. Take the time to clean up these areas and you'll end up with a nice fuselage.

Window and door openings need to have the edge curves extracted and can be projected onto the base fuselage to trim out. Same with areas where graphics are to be applied.

Tim Flater
NX Designer
NX 9.0.2.5 Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB

 

[MichaelkSA]

Thank you all for your replies.

Cowski, I did indeed change the tolerances after creating the 'sew', so I will try to redo that process although from the comments after yours it seems like I still have some work to do on the geometry before that will work.

Tim, the stuff you propose is a bit advances for me as a new NX user but I will give it a try. Thanks.

A final question on the topic. After I have created a solid body. Is it possible to save that body as a single part file without all the part 'history' going along with it? Basically so that i can have a 'clean' part that i can pass along to other people without them needing to see exactly how I got the part to be as it is.

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[Xwheelguy]

Regarding your final question, Edit -> Feature -> Remove Parameters to remove all history. When using this method, careful not to overwrite your model with history by doing a Save - use Save As. IMO, the safest method is to Export Part and tick the Remove Parameters option near the bottom 1/3rd of the dialog.

Tim Flater
NX Designer
NX 9.0.2.5 Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB

 

[MichaelkSA]

Great thank you very much Tim.

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[ARZinAZ]

It appears the problem surfaces are near the pitot/static ports under the aft cockpit windows at about station 131 and at the interface of the forward edge of the aft horizontal stabilizers at about station 1025.

Notice if you create a solid block and use the fuselage faces to trim that block into a tube it works fine as long as the block starts aft of 130 and forward of 1020. Use this method to subtract a solid from the trouble spots and remove the parameters and see if deleting the faces of the block you subtracted from the sheets to heal the face.

Let us know how it goes.

 

[MichaelkSA]

That is a clever method. I will give it a try, thank you!

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