Cancel
Showing results for 
Search instead for 
Did you mean: 

Temperature Loads question

Experimenter
Experimenter

Hello everybody! i am having this problem from long time ago so today i got the courage to ask you guys . (if my question is too stupid please know that i'm a beginner)

I applied a Temperature load (on nodes) of 700 degrees CELSIUS on a 1000x1000mm plate, 8mm thick  , the body load was 30 degrees CELSIUS . The plate was constrained at the top and the bottom (fixed constrains).I did a static analysis then showed Untitled.jpgelemental contour Smiley Tonguelate top vonmises stress. the material is the stock one that we find in FEMAP , AISI 4340 Steel . after i select the views i get the legend on the right side of the screen . can you help me telling what the results are in ? are they n/mm2( way too big tensions)? what are they?

3 REPLIES

Re: Temperature Loads question

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

Dear Mike,

CAUTION!!, you have the worst problem of FEMAP, mixing units!!.

I realized of this because the material name AISI 4340 STEEL only exist in the MATERIAL.ESP file, that is the default material library, but values are in INCHES & POUNDS!!.

This means that you have a serious problem of configuration, go to FILE > PREFERENCES and set as minimum two changes: geometry & material library (see my website in the following address: http://www.iberisa.com/soporte/femap/femap_tips_tricks_preferencias.htm):

GEOMETRY: this option affect when you import any CAD model (Step, Parasolid, IGES, etc..) in FEMAP, choose "2..Millimeters" to get the length of geometry scaled to millimeters.

 

femap_tips_tricks_preferencias_geometry

 

LIBRARY/Startup: for MATERIAL choose the file "mat_eng_mm-N-tonne-degC-Watts.esp", units there are consistent to have the geometry length in millimeters.

 

femap_tips_tricks_preferencias_library

Regarding the units of the stress results of your problem if you choose from the new library a steel material say "AISI Carbon Steel 1006 Cold drawn" please understand the following:

• Young module value, EX = 199948 MPa.

• Coef. Themal Expansion, AlphaX = 1.512e-5 /ºC

• Temperature Reference, Tref = 21.1 ºC

material-steel.png

Tref =21.1ºC is an important value, it means that at 21º.1ºC we have a zero strain state. The thermal strain is proportional to the temperature change x linear coef. of themal expansion, EpsilonX = AlphaX * DeltaT. Then if you apply a nodal temperature of 700ºC and your Tref=21.1ºC then DeltaT=700-21.1 = 678.9ºC, OK?.

The next plot shows the thermal stress results, of course, units are MPa (ie, N/mm2). Of course, in real life the material never will reach that stress value, the material yields, but is important to understand the consequences of fully constraining structures, when thermal loads are present then inclusion of thermal joints to account for free dilation is critical!!.

thermal-stress-result.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: Temperature Loads question

Experimenter
Experimenter
Thank you so much for helping me !

Re: Temperature Loads question

Phenom
Phenom
If you need a summary doc on consistent units, just google Femap Consistent Units
The endurasim pdf covers the topic quite extensively for both heat transfer and mech.