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Sheets to Solid Bodies

Sheets to Solid Bodies

Sheets to Solid Bodies

(OP)
Hi NX'rs,

  I have 4 sheet bodies with unique profiles.  I now want to make a solid body either directly from the sheet bodies or use them to cut the final profile.

  I "sewed" the sheet bodies together, but don't recall on how to make a solid body.  Creating another solid body & using the sheets to trim does not seem to be working.

  What's the process to create a solid body from the sheets or to use them as cutting tools?

Thanks
 

RE: Sheets to Solid Bodies

If you sew the sheets together and they form a 'watertight' body, then the result will automatically be a solid.  

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/

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

RE: Sheets to Solid Bodies

(OP)
Hi John & Others,

  I have 6 sewn sheet bodies - 4 sides & top & bottom.  Visiually, it looks o.k, but they're still not a solid body.

I've submitted a CAD file for example.

  I attempted to upload a NX 7.5 file, but it's not able to upload at this time.  I'll have to try again later.

Thanks
 

RE: Sheets to Solid Bodies

Before you go any furture, go to...

Preferences -> Modeling -> General

...and check to make sure that the 'Body Type' option is set to 'Solid'.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/

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

RE: Sheets to Solid Bodies

(OP)
Hi John,

  My preferences aren't the issue here in that they are already set to the suggested settings stated above.

  If I click in the "sew" feature, all sheet bodies (walls - sides & top & bottom) highlight as they should be.  However, it's still a bunch of (connected) sheet bodies.

 For whatever reasons, I can't upload my CAD file either, otherwise I would submit for review.

 

RE: Sheets to Solid Bodies

Run examine geometry and check for sheet boundaries. This will highlight areas where the edges of the sheets don't meet.

RE: Sheets to Solid Bodies

(OP)
Hi Guys....

  The Examine Geometry check doesn't highlight any issiues or discrepancies.  

  What might be the other causes?

 

RE: Sheets to Solid Bodies

What method/command are you using that reports it as sheet bodies?

RE: Sheets to Solid Bodies

Why are you even sewing sheet bodies together?  This is the sort of thing which can be produced using the Swept Solid function where it's created as a solid body in a single operation.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/

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

RE: Sheets to Solid Bodies

(OP)
Hi John,

  As you can kind of see in the pics, this area has a couple of transition & twist areas.

  Initinally, I thought the Through Curve or Through Curve Mesh features would define this area well, but as you can see, some areas becomes "funky" & gives undesirable results.

  At this point, I've tried a 100 different ways from creating a solide then, using the sheet bodies to trim to whatever else.

  Each process works to a degree, up until that point where I can't control & cant' get my desired solid body geometry.

  Obviously, I'm doing something wrong here... I've done similar jobs in the past & didn't have these many issues....

  Whatever works - That's the answers I'm seeking...

Thanks again for the assistance...

 

RE: Sheets to Solid Bodies

Can you just upload the model consisting of the curves and NOT the solid/sheet bodies?

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/

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

RE: Sheets to Solid Bodies

OK, here's my first cut at this using Swept Surface with 2 Guide curves (I've only included the curves and objects needed to define this body).

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/

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

RE: Sheets to Solid Bodies

(OP)
Hi Everyone,

  It took me to two dam days & a lot of trial & errors, but somehow, I finally got my sheet bodies to become solid bodies.

  However, the geometry is still not perfect, but it's not horrible either.  

  I used the Through Curve Mesh feature & made 2 halves.  Previously, I was sectioning these into 4 walls.  For the most part, this seems to work, but for whatever reasons before, it didn't.


 Now, if I could figure out on how to get "cleaner" geometry that doesn't over revolve & give a "hump" appearance...

Any suggestions....???

RE: Sheets to Solid Bodies

(OP)
Hi John,
 
  You make it look so easy.... I know I tried something similar several times & I did or still not get the same "desireable" results as you did.

  I tried to duplicate your processs, using the same settings, line type selection - Tangent & vector direction.  However, my solid faces are resulting in very choppy faces.

  See attached pic.

I'll try again in the morning...


 

RE: Sheets to Solid Bodies

(OP)
Hi John,

  I noticed you added a Datum Coordinate System in your example, which is something that I don't have in my model.  

What does this do?

RE: Sheets to Solid Bodies

back to the sewing issue. When I have trouble sewing surfaces together some times I can get it to work by adjusting (increasing) the tolerance value.

RE: Sheets to Solid Bodies

Quote (REDesigner09):


I noticed you added a Datum Coordinate System in your example, which is something that I don't have in my model.  

What does this do?

Nothing!

The method I used to get a part file which ONLY contained the information needed to model what I had was to export the solid body and all if references to an empty Part file which already contained the Datum CSYS since my Modeling template files all have a Datum CSYS as the first entity just in case I need to for reference when I start constructing something.  In this case, it was just there by default and added nothing to the solution.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/

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

RE: Sheets to Solid Bodies

(OP)
Hmm?

  As far as I can tell, I'm duplicating your process & yet, I'm clearly not getting the same results.  Therefore, I guess I'm not duplicating your process.


  Is there a specific process that I should be following?  I know NX can be sensitive to pick selections, line entity types, etc., but considering this is all from my my model, this shouldn't be an issue.

Thanks
 

RE: Sheets to Solid Bodies

OK, take the model I uploaded and delect the solid body and start over.  Rotate the model around so that the two Green 'Guide' curves are displayed as being on the 'front' of the model.  Now using 'Swept' feature, select multiple 'Sections' (one at a time) using 'Tangent Curves' selection intent, by starting your pick at the end of the long curve near the Left 'Guide' curve.  Under 'Section Options' set Interpolation to 'Cubic', Alignment Method to 'Arc Length' and Scaling Method to 'Uniform'.  In the 'Settings' section, set the Guides Rebuild to 'Manual' and the Degree to '5' and the (G0)Position to '0.001'.

Anyway, give it shot.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/

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

RE: Sheets to Solid Bodies

(OP)
Hi John,

  So, this is the trick!  I need to change my 'Section Options'.

  I'll have to check this when I get back to work.

Thanks agian...
 

RE: Sheets to Solid Bodies

(OP)
Hi John,

  I changed my Selection Options as instructed, however, I'm still not quite getting the results you got.

  Compared to before, It's much "cleaner", but the top half of my solid, where the majority of my sections are, is coming out a little rigidity.

  I had no problem duplicating your process in your model, but for whatever reasons, something is still different in my model.

  I'm selecting my sections from the bottom-up

  Selected my two guide curves & changed my selection options.

  However, NX is instructing me to first select my orientation, which I simply selected the guide curves.

  Then in the Scaling Method area, I am not initially getting the "Uniform" option.  Instead, I am getting:

  Constant
  Blending Function
  Another Curve
  A Point
  Area Law
  Perimeter Law

  I kept the Constant option.

  Changed the Guide area to Manual & Degree to '5'.

 The result is a solid that is kind of rigidity.

  If I edit my the Swept feature, then it displays "Uniform" in the Scaling Method area.

  How can I remove the "rigidity" appearance?

Thanks again...

RE: Sheets to Solid Bodies

Did you set alignment to 'arc length'?

RE: Sheets to Solid Bodies

(OP)


Yes - That was an option available that I selected.
 

RE: Sheets to Solid Bodies

Quote:

Then in the Scaling Method area, I am not initially getting the "Uniform" option
You won't get the uniform/lateral scaling option until you have selected 2 guides.

Are the arrows on all your sections pointing the same way? If not, use the reverse button on the oddball section(s).

If this doesn't fix it can you post another .jpg?

RE: Sheets to Solid Bodies

I can't open John's file (I'm still on NX6) but take another look at his file. At a guess, I'd say he didn't use as many sections as you did.

RE: Sheets to Solid Bodies

I'm curious, did you find the solution?

RE: Sheets to Solid Bodies

(OP)
Hi,

  Thus far - No!  

As far as I can tell, John used the same sketch or line entities that I submitted from my CAD file.  We have the same guide point locations & my cross-sections are from the bottom-up, with the vectors point in the same directions.

  My select options are now the same, as far as I can tell, which they weren't before.  

  However, for whatever reasons, part of my solid is coming out "rigidity".

  I'm not sure if this is not a graphics thing, but I don't expect that being the issue.

  The Design Intent was to layout a handful of cross-sections, then be able to sweep those cross-sections in some way to make a nice "clean" parametric model.

  Thus far - That's not working...
 

RE: Sheets to Solid Bodies

Can you get an acceptable result if you take out some of the sections? The combination of a cubic fit and lots of sections makes for 'burples'. Think of fitting a polynomial through X,Y point data - you potentially end up with lots of inflection points to get the curve to smoothly pass through all the points. That's what NX is doing, except in 3D. Less sections will result in a smoother solid.

If you really need it to pass through all those sections and be smooth, you may need to try plan B. Build it in sections. Use swept along with the bottom 3 sections and top 3 sections and use a command such as through curves or through curve mesh (that allow you to define tangent conditions) for the middle part(s).

RE: Sheets to Solid Bodies

(OP)
Hi Cowski,

  I cold do this, but then I loose some of the profile that I need to contrain to.  In areas where I don't pick my cross-sections, the solid will eithe result as being over or under - or a combination of both around the cross-sections.

  This area is almost like an airfoil where I have to keep a specified profile all the around.  I cannot deviate from this if it's not within tolorance.
 

RE: Sheets to Solid Bodies

I don't see what the problem is?  I've all but provided a step-by-step written description of what I did.  All you have to do is EDIT my SOLID body and look at the settings in the dialog.  You will see exactly the options and values that I used when I created the solid.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/

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

RE: Sheets to Solid Bodies

(OP)
Hi John,

  I don't see what the issue is either.  I "think" I did what you did & have my preferences the way you have & yet, as you may have seen in my pictures, part of my solid is coming out "rigidity".

  I'm still reviewing, but at the moment, I can't find anything. Perhasp, we have a virtual meeting through Teamviewer or something.

  I'm also on the Pacific Coast, so we can schedule.

Thanks
 

RE: Sheets to Solid Bodies

Perhaps, but technically I'm on vacation until January 5th, 2011 and so I'm 'working' from home where my network connection is not always the fastest.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/

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

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