Cancel
Showing results for 
Search instead for 
Did you mean: 

meshing

Pioneer
Pioneer

please see the atttached meshing on a surface seperated by curve.. i gave meshcontrol as 50mm mesh size on surface for both surface and meshed both with same property, the meshing is not coming smooth across the curve - please help on why its not coming proper.

15 REPLIES

Re: meshing

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

Dear Rajith,

If you issue command "Modify > Color > Solid > Method=ALL" and select a color and click in RANDOM you will see by color that different solid bodies exist, then you have "duplicated" curves at each intersection, each one with different element size. Also, you can see that duplicated sheet body exist, just in top of each other. Then this explain why you don't have for sure mesh continuity between different surfaces, because they are independent!!.

 

duplicated-surface.png

 

Then I suggest first at all to delete the redundant surface and then use command "Geometry > Surface> NonManifold-add" to stitch all surfaces in ONE NonManifold Sheet body to make sure that only ONE curve will exist between neighbour surfaces. Please note to make sure to set OFF the option "Incremental Checking" also use a tolerance of 1e-4. The result is the following: in yellow color you will see the free edges!!. This way mesh continuity between surfaces is assured!!.

 

non-manifold-add-tolerance.png

 

non-manifold-add-free-edges.png

 

Now you can perform in FEMAP a Shell mesh with CQUAD4 elements with the best quality possible, see below:

 

CQUAD4-meshing.png

 

Enjoy!!.

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: meshing

Pioneer
Pioneer

hi,

thanks a lot Mr. Blas Molero, 

 it solved my meshing issues.. i am on half way with the model(attached here) i applied a horizontal load at one end of the column, and gave fixity at one end of the column and ran a linear static analysis, i see the stress occurs only for the cell/node where the loading is applied and is not getting transfered elsewhere. ..capture-01 attached here shows that the load is applied along the perifery and the stress occurs only at this location...could you please look into this... thanks for your support. looking forward to hear from you - will be great help considering my urgency.

the model is available on this link as the size was big

https://drive.google.com/file/d/0B9gSrTCMo9R3Rm9VOXBocnRHRVU/view?usp=sharing

 

 

Rajith

Re: meshing

Pioneer
Pioneer
Mr Blas Molero, the link to download model is not working in earlier mail, please find the updated link. https://drive.google.com/file/d/0B9gSrTCMo9R3aEZZRWZSZi1yX1U/view?usp=sharing thanks Rajith

Re: meshing

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

Hello!,

First at all you need to improve your mesh quality, you have a problem: the mesh continuity is not assured!!.

 

FREE-EDGE.png

 

To see the free edges together with mesh & geometry click in F6 > tools & view style > Free edges & faces ...

 

view-free-edges.png

 

If you solve your mreshing problems and run the analysis you will see the following vonMises stress results:

 

postprocessing-results.png

 

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: meshing

Pioneer
Pioneer

thanks Mr. Blas for your quick reply,

 

but i think you used the model which i send in the earlier link for which i send you another mail/link with updated model and for that model, i am not getting deflection as expected. please see the video(uploaded as attachment) showing the way it happens when i hit the deflection mode.

 

 

the model(updated/no free edges) is available at following link(also in previous mail)

https://drive.google.com/file/d/0B9gSrTCMo9R3aEZZRWZSZi1yX1U/view?usp=sharing

Re: meshing

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

Hello!,

Make sure to active the correct Output Vectors and you will arrive to similar results to my plots. Using you lastest link here you are the results I use:

 

postprocessing-results#2.png

 

Click in COUNTOUR OPTIONS and make sure to activate elemental results, use corner data, etc.. Also activate DOUBLE-SIDED planar contours.

 

postprocessing-results#3.png

 

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: meshing

Pioneer
Pioneer

thankyou Mr. Blas, i tried this, and my deflection pattern looks ok (cantiliver deflection under point load). but the stress distribution appears to be very local. please refer to the uploads.

 

thanks for you support

 

Rajith

Re: meshing

Pioneer
Pioneer

Mr. Blas, thanks for your help. i am attaching my full model with this, the screenshot 'fig-1' attached here shows the full column under study modelled partly with plate element and then continued as a single tube element and they both mated with RBE2 element. loading is applied at two locations and the deflection is also uploaded along with the model. could you please tell why the tube tip (free end where loading is applied) is not showing any defleciton in the model, also why the deflection in happening locally at the mating location.

model location

https://drive.google.com/folderview?id=0B9gSrTCMo9R3eXZUU0Vkbk9tQmM&usp=sharing  

 

 

thanks once again.

Rajith

Re: meshing

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

Dear Rajith,

The CTUBE element is the same as the CROD element except that its section properties are expressed as the outer diameter and the thickness of a circular tube, then it has only axial and torsional stiffness, so the result you see in the screen are reasonable according your selection. Please use a genuine beam element, for instance CBEAM, to capture bending stiffness!!.

 

Also, please do not mesh the colum with millions of beam elements!!, for linear static analysis (SOL101) is useless, this is a "discrete" beam element where displacement & stress results are not mesh dependent, the solution is exact not matter you mesh with 10 or 1000 elements, OK?. For Beam elements the common engineering sense is to use an element size of say two to four times the beam cross section dimmension (well, in modal & buckling problems you may want to increase the number of divisions to capture correctly the mode shape with minimum six element divisions per sine!!).

 

And finally, I strongly suggest to Update your FEMAP version, I note you run old V10.3.

Good luck!.

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/