you mean that i have to declare the poisson coefficient value to perform my analysis ? the stress remains the same if i just change the young's modulus ?
In static analysis (for statically determined structures and maybe for static indeterminate structures made from one material because stiffness ratio remain the same) stress don’t depend from material properties. For tension/compression stress is F/S, where F is force and S is area, for bending stress is M/W, where W is moment of resistance - there are no E in this calculations. Poisson ratio is not the value, that you can change free. The difference between steel and copper is that some stress is allowable for first and not allowable for second material. Usually engineers change geometry of structure, add some new parts to resist force, or select harder material with higher allowable stress. Engineers are not wizards and they can`t change poisson ratio of steel from 0,3 to 0,45 or 0,1) So if your structure with S235 steel is fails then select S355 steel.
Stress is independent of Modulus of Elasticity but depend on geometry and force.(σ =F/A). If you take three rods of same area A but of three different materials and apply same force F, what will be the stress? Stress will be same but deflections will be different(δ=(Force*Length)/(Area*Modulus) since modulus is different.
In FEA, you will get the different deflections due to change in Modulus but stress will remains same since you have not changed area or force. Software first calculates the deflections but modulus remains neutral to calculation.
(σ=E*ε=E*(Force/Area*E)=Force/Area)
Now you can ask your colleagues a tricky question:
"I have two rods with 1 cm^2 cross section area, one made of steel another from cooper. Tensile force of 100 N applied to both rods. Where the stress will be larger and where smaller?"
The simple answer is stress will be equal.
More precise answer is stress in copper rod will be larger, but difference will be very very very small.
P.S. Hivemind in eng-tips)
Thanks very mush to this replies,So to simulate the stress intensity on my model in differents case of temperature, i have to perform a structural and thermal analysis (i can't just take acount the modulus young.
please find attached the screen of my model and give me your point of view ( 3 cases of temperature nedeed 100 , 230, 350)
You can. If your detail has uniforn temperature distribution - all material is 100 or 230 or 350 C at diferent cases, then you will have same stress but different deflections. In linear theory you can even calculate deflections for different E by hand from one case solved in FEA. For example point of structure have 1 mm deflection at E=200 GPa, so an 100 GPa it will have 0,5 mm deflection - all is linear. Thermal stress appear only if detail have temperature gradient or thermal expansion of structure is constrained, If you put bolt into and slowly heat it will dont have thermal stress neither at 20 C not at 1000 C.
I undrestund you but in my case i want to simulate other type of stress like bending stress and membrane, so it will be complicated.
I can perform thermal (uniform temperature) + structure analysis in order to determine this type of stress ?
because i tried and it gived me high stress value (what i have to check ?).
please find attached the screen to undrestund what i mean.
Bending, membrane and other stress in linear formulation also dont depend from E, only from geometry. Post here model to see what is constraints of detail. All your model is blue, the hot spot mau occure at constraint point or due to singularity - in both cases you can neglect this stress because it is nonphysical.
you find the model in the attachement, the structure is constraint for Moving in all the directions (surface below of the horizantal plate), and a force of -1000N is applied on the round shape of the vertica plate.
i need to simulate the membrane + bending stress in 3 case of temperature as i said previously.
By model I mean worckbench project archive, not a picture. If high stress occurs an constraint during thermal stress analysis it is ok. You prevent nodes on surface from moving and gt large stress. Just dont look at this part of model, change magnitule of stress in legend, recal Saint-Venant's principle Link or model real conection of model to ground - only superman can hold plate at temp 350 C and plate dont change it geometry. What is physical description of your bromlem - the model is bolted or welded? Maybe model can expand due to some small clearance in connection? And maybe constrained part is not the point of interest. try to constrain one corner and allow surface to slide in horizontal plane. Also ground structure isnt absolute rigid and expand due ti temperature together with detail, isnt it.
You tried)
Run command File->Archive, wbpj file is only index of geometry and mesh files and uncheck option Results/solution to minimize file size.
As for your problem - what is the point of interest - stress and displacement due to force - then you can calculate three values of E for each temperature or in addition, you want to see stress/displacement condition at lower surface?
In first case, you can neglect thermal stress near constraints because it is nonphysical.
In second case, you must model real connection between detail and ground, you must model some portion of grounding structure - move boundary conditions far away from zone of interest - it is one of basic principles of FEA, CFD and all computational physics, as I say Saint-Venant's principle.
Better, make simple model, if you have some privacy issues, and post in here, better to solve problems together.
I`m 95% sure that you don’t need thermal load - use different E. However, I can only suggest. Nobody know the problem better than you.
