Cancel
Showing results for 
Search instead for 
Did you mean: 

Bolt Preload Errors

Pioneer
Pioneer

Hi All,

 

I am trying to use bolt preload and getting errors. I am not sure if what I am doing is 100% correct. I made the lower plate as rigid and the upper bracket as deformable. I applied the preload but it says that i have not applied any bolt forces. Do I need anything else to make the simulation run?

I am not sure about the steps I followed. It would be helpful if somebody can guide me through this.

 

Also, does it have to be a non-linear static analysis or would linear static work?

I have read that working with bolt preload requires two non-linear analyses in a row but I am not sure I got that.

 

I have attached a png file.

 

Thanks,

Bhumika

10 REPLIES

Re: Bolt Preload Errors

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

Dear Bhumika,

Take a look to this tutorial:

http://www.iberisa.com/soporte/femap/tornillos_pretensados_chexa8.htm

Without the model in hand is difficult to know the reason of the error.

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/

Re: Bolt Preload Errors

Pioneer
Pioneer

Hey Blas,

 

I am not able to share the file since it is bulky.

 

Thanks

Re: Bolt Preload Errors

Siemens Phenom Siemens Phenom
Siemens Phenom

From your snapshot, I cannot see where the model is constrained. 

 

In addition, it appears that you have a thin body meshed with only one layer thick of solid elements.  That will be an overly stiff model as it will not yield reliable results in bending.  You should model this will shell elements that will results in less nodes and a more accurate result.

Best Regards,
Chip Fricke
Principal Applications Engineer - Femap Product Development

Re: Bolt Preload Errors

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

Dear Bhumika,

Simply delete ALL results of the FEMAP model and do a FILE > REBUILD, and next save your FEMAP model, now you will see that the model size is very reduced, very small, simply ZIP the file and post it here, 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/

Re: Bolt Preload Errors

Pioneer
Pioneer

Hey Blas,

 

Please find the attachment.

 

Thanks,

Bhumika

Re: Bolt Preload Errors

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

Hello!,

Well, you have severe errors in your FEMAP model, you have used wrong concepts in meshing, element type, contacts, and loadings:

  • First the mesh: this is a 2-D plate problem, then the use of Shell meshing + midsurfacing is the correct meshing approach. You have created a 3-D solid mesh using TET10 elements, but used only one element in the thickness, and this is not correct from the point of view of stress accuracy, with solid eleents to properly capture the stress gradient in solid walls you need to mesh with minimum two elements in the thickness. 
  • Regarding bolt preload: you have created one 1-D CBEAM element using the API "CUSTOM TOOLS > MERSHING > HOLE TO-HOLE FASTENER". Good, this is more proper for SHELL meshing, with solids is better to select nodes on the washer, but OK. Later you define a BOLT REGION using the faces of the 3-D solid elements: wrong!!. 

bolt-preload1.png

Here this is what you do bad: you define a bolt region using bolt type = beam/bar elements, good, but later you select the faces of the 3-D solid elements insted the previously created CBEAM element, and this is wrong!!.

 

bolt-region0.png

bolt-region1.png

When working with beam elements to define the bolt is not necessary to define any BOLT REGION, FEMAP will do the job for you automatically: simply use command MODEL > LOAD > BOLT PRELOAD and select the option ELEMENTS and enter the value of BOLT PRELOAD. Next FEMAP will ask you to select the CBEAM or CBAR element representing the bolt, and FEMAP will define the BOLT REGION for you, OK?.

bolt-preload2.png

Regarding contacts you have defined a SOURCE REGION using ALL SURFACES of the bracket: wrong!!. The idea when selecting a contact regions is to define the SOURCE & TARGET regions in contact based in the touching surfaces, not the parts, OK?.

connection-region.png

For the SOURCE REGION simply define the bottom surface of the bracket, and for the TARGET REGION simply define the top surface of the rigid plate. By the way: in the definition of the region do not use the option RIGID, use always DEFORMABLE, this is linear contact analysis, the RIGID option is for more advanced analysis.

If you run this way then you will arrive to a valid solution, here you are:

bolt-preload3.png

here you are the model in FEMAP neutral file format for version 11.3.
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/

Re: Bolt Preload Errors

Pioneer
Pioneer

Thank You, Blas

 

That was a lot of help. 

 

I have one more question. When I apply preload to the beam element, it asks me for the loads on the elements. So what kinda load are we talking about in here. Because the only load I have is G-loads which are the body loads for my structure. 

 

 

 

Re: Bolt Preload Errors

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

Dear Bhumika,

Bolt Preload command simply ask you to select the beam elements that form the bolt where to apply the bolt preload. If you mesh a bolt with more than a CBEAM or CBAR element, simply choosing one individual CBEAM or CBAR element is enough, not need to select all.

If you choose multiple elements to apply Bolt Preloads, FEMAP will combine any selected elements which are “connected” into a single bolt region. This is actually very useful when creating Bolt Preloads as you can choose all of the Beam or Bar elements in a model. In this case, each “connected set” of beam/bar elements will become and individual Bolt Region with appropriate Bolt Preload.

You can mix bolt preloads with any service loads, like Gravity accelerations, pressure, etc.., 

Bolts (and certain types of threaded fasteners) are commonly tightened to levels producing very high preload forces. Preloading bolts to about 75% of their proof strength is typical. The bolt preload capability in NX Nastran solver allows you to predict stresses in the bolts and the bolted medium that arise from bolt preload forces alone or bolt preload forces and service loads.

Historically, bolt preload was modeled using either an equivalent thermal load approach or a multipoint constraint (MPC) approach. Both methods are capable of providing accurate results. However, both methods are labor intensive requiring multiple solutions, manual capture of data, and hand calculations.

The NX Nastran approach is much more efficient because the entire run is automated and allows for direct entry of the bolt preload forces. During the run, the model is solved twice.

  • The first solution calculates the deformed shape of the bolted medium resulting from bolt preload forces. The software then performs an intermediate calculation. The appropriate compressive forces to apply to the bolts during the second solution are calculated correcting for differences in the length of the bolt model and the loaded length of the actual bolt.
  • Solving the model a second time gives the stress state resulting from bolt preload forces and, optionally, service loads.

Bolts can be modeled using 1-D CBEAM and CBAR line beam elements or alternatively 3-D CHEXA, CPENTA, and CTETRA solid elements. And bolt preload is supported in SOLs 101, 103, 105, 107 through 112, and 601.

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/

Re: Bolt Preload Errors

Pioneer
Pioneer

Hi Blas,

 

When I get the option for creating loads on the element, there is no option for acceleration.

 

The image below shows the only option I get.