turn on suggestions

Auto-suggest helps you quickly narrow down your search results by suggesting possible matches as you type.

Showing results for

- Navigation
- Simcenter
- Forums
- Blogs
- Knowledge Bases

- Siemens PLM Community
- Simcenter
- CAE Simulation - NX Nastran Forum
- Press fit simulation

Options

- Subscribe to RSS Feed
- Mark Topic as New
- Mark Topic as Read
- Float this Topic for Current User
- Bookmark
- Subscribe
- Printer Friendly Page

Highlighted

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

02-19-2015 06:16 AM

Hi Everybody,

I have been using NX for about 8 months now. I was doing more thermal analysis and simulations and now I want to perform some structural analysis. I am working right now on a plastic enclosure that will be assembled with press fits. the inner part of the hub will have an hexagonal shape and the shaft is cylindrical. So far I have not been able how to simulate a situation when the assembly is being done.

I have used a enforced constrain to make the pin move in the direction of the hub but it stops when it reaches the entrance of the hub. I am assuming the problem is how I am using the surface to surface contact.

I assume someone has already done something like this so if any of you guys has some suggestions I will be extremely thankful

Thanks for your support

Cesar

Solved! Go to Solution.

Labels:

12 REPLIES

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

02-20-2015 08:30 AM

Cesar,

You are analyzing the assembly process correct? NX Nastran advanced nonlinear (solution 601) is what you would want to use for that type of problem. With that solution you can define a transient enforced displacement such that you step through the assembly process. With linear statics, you have the ability to define a single load condition (or just 1 step) and it will not provide the solution you desire.

Regards,

Mark

Mark Lamping

Simulation Product Management

Product Engineering Software

Siemens Industry Sector

Siemens Product Lifecycle Management Software Inc.

mark.lamping@siemens.com

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

02-21-2015 06:27 AM

Dear Cesar,

If you want to simulate a "**Interference-Fit**" problem then you can run linear elastic contact stress analysis (SOL101, i.e. the stresses should be smaller than the elastic limit Rp0.2 of the materials) (see my post here: https://iberisa.wordpress.com/2012/01/16/tratado-completo-sobre-como-resolver-problemas-lineales-de-... ) or if you have large displacements & large strains (snap fit is not small) the you will have to run advanced nonlinear analysis (SOL601) as Mark suggested.

Remember that you will need to define a negative search distance for contact in the BCTSET card to solve the material penetration (ie, interference-fit) between parts using a value bigger that the interference. Also the INIPENE=0 should be used in the BCTPARM card to solve the initial penetration.

Of course, in the previous approach the interference fit should be modeled explicitly in both the geometry & mesh. Alternatively you can use OFFSET distance for contact regions that will allow you to neglect the interference at the geometry level and use the same same geometry dimension for both contact parts.

But reading your description it seems you have a interference fit problem between a cylinder and a hexagonal hub, so first approach will run OK for you.

Best regards,

Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

10-21-2016 10:52 AM

Dear Blas,

The INIPENE should be set to ''Calculate from geometry'', if not the software will consider as there is no ineterference between parts. I tried to set INIPENE to zero and the results were like there is no ineterference between parts.

Best Regards,

Yousef

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

10-21-2016 06:02 PM

Dear Yousef,

**INIPENE=0** means "**Calculated from Mesh".** The INIPENE field on the BCTPARM entry controls how NX Nastran handles initial gap or penetration of the generated contact elements. No corrections will occur for gaps or penetrations (Default = 0).

Whe **"0..Calculated"** is used the NX Nastran software evaluate contact exactly as the geometry is modeled, and if penetration is found then it will be resolved. In the case of penetrations, a model may experience “press fit” behavior when using this option.

If you need to solve a "press fit" problem, then use INIPENE=0.

Best regards,

Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

10-23-2016 10:00 PM

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

05-14-2017 11:20 AM

Hello,JimB,

One question for press fit assembly,

What is your mean for "target and source meshes match exactly" ?

Does it mean there is no interference for mesh ?

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

05-14-2017 04:04 PM

Dear Pioneer,

If the mesh is not "exactly" coincident between nodes in source & target region, then the chance to suffer undesired initial interference (overlapping) is a risk, specially when using low-order elements like 2-D plate CQUAD4 4-nodes or 3-D solid CHEXA 8-nodes. Using high-order 3-D solid TET10 elements with midside nodes moved to surface geometry then eliminate the problem. But the best advice I can give you is to use always matching mesh, not matter if using low or high-order elements, OK?.

Best regards,

Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

05-16-2017 10:35 AM

Dear BLas,

one point I am not so clear,

because source faces have different size (such as different diameter) for press-in assembly,

how to realize matched meshes between source and target surface in NX ?

Best Regards,

Wanghua.

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

05-16-2017 11:00 AM

Dear Wanghua,

Easy, simply split surfaces in the idealized environment to have regular surfaces, this way you can generate a structured mesh controling the same number of elements in both parts. Use command **2-D MAPPED MESH**, or 2-D FREE MESH activating the option** ATTEMPT FREE MAPPED MESHING** and prescribe local mesh controls to have the same number of elements.

Best regards,

Blas.

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

Follow Siemens PLM Software

© 2019 Siemens Product Lifecycle Management Software Inc