units
units
(OP)
I am really confused about units. For my abaqus part i am using mm, for load N, (thus pressure loadings are N/mm2), and thus as i had read on a thread here density is in tonnes/mm3 to keep the Newton consistent. Now, when i input a hyperelastic material via stress strain data values (uniaxial) do the stress values have to be converted to N/mm2 or not? thanks
andrearrd
andrearrd





RE: units
corus
RE: units
If your part is in mm, your density can be specified in kg/mm^3 and any gravity loading specified in m/s^2 to maintain consistent Newton loading. A good way to always check your units is to look at Newton's second law, F=m*a:
F = m*a = rho*v*a = (kg/mm^3)*(mm^3)*(m/s^2) = kgm/s^2 = Newton
where 'rho' is mass density, 'v' is volume and 'a' is acceleration.
Pressures hence are in N/mm^2 - all consistent.
-- drej --
RE: units
RE: units
F = m*a = rho*v*a = (T/mm^3)*(mm^3)*(m/s^2) = Tm/s^2 = Newton*1000 = kN
If you use both Tonnes and mm/s^2 with mm dimensions, those units would be a real pain to convert to 'standard' notation.
Furthermore, if your acceleration is in mm/s^2 your force unit will be kN:
F = m*a = rho*v*a = (kg/mm^3)*(mm^3)*(mm/s^2) = kgmm/s^2 = Newton*1000 = kN
Personally, I always try and use units which don't require coefficients to maintain their consistency i.e. I always use Newton-Metre-kg or Newton-Millimetre-kg. This way you avoid tying yourself in knots.
RE: units
F= m*a=rhoe*V*a=(kg/mm^3)*(mm^3)*(mm/s^2)= kg mm /s^2
as u say above, and thus all my forces would be in N/1000 . If i wish them to be in N then is it not ok to simply input the density as tonne/mm^3 since:
F=m*a = rho*V*a= (T/mm^3)*(mm^3)*(mm/s^2)=T*mm/s^2= kg*m/s^2 = N??
This is waht Corus had said in an earlier post and it makes sense to me.
Thanks,
Andrea
RE: units
You said:
".. If i put kg then
F= m*a=rhoe*V*a=(kg/mm^3)*(mm^3)*(mm/s^2)= kg mm /s^2 as u say above, and thus all my forces would be in N/1000 ."
How do you obtain N/1000 from this?
Secondly, how do you get:
F=m*a = rho*V*a= (T/mm^3)*(mm^3)*(mm/s^2)=T*mm/s^2= kg*m/s^2 = N
in particular the T*mm/s^2= kg*m/s^2 = N?
Shouldn't this be:
F=m*a = rho*V*a= (T/mm^3)*(mm^3)*(mm/s^2)=T*mm/s^2= kg*1000*m*1000/s^2 = Mega Newton
As I said earlier, if you use mm and you want Newtons as your force, your density should be kg/mm^3 and your acceleration m/s^2. It's as simple as that.
RE: units
corus
RE: units
Drej unless im making a silly mistake isnt it:
T*mm/s^2= kg*m/s^2 = N since 1T=1000kg and 1mm = 0.001 m therefore T*mm/s^2= 1000kg*0.001m/s^2 = 1N
and luckily i dont have to do a thermal analysis!
Thanks,
andrearrd
RE: units
As a footnote, density is not entirely irrelevant in a static analysis - it is in the inertial sense - as this becomes important when gravitational loads (body accelerations) are applied statically.
Cheers,
-- drej --
RE: units
thanks again
RE: units
If your "loading rate" is correct, then the inertial effects you're seeing will be correct will they not? If you want to speed the analysis up without influencing your results too much, you can do a number of things. First of all, try "mass scaling". Just increase the mass density throughout your model by a factor of 10 and check the results to see if you get any artificial inertial effects - if not, increase by 10 again and so on. You'll find quite an improvement on analysis time. Be careful about your load though, as initially the loading rate you apply should match that in the physical system (to check for effects of this load) - especially if it is applied quickly or relatively quickly with a large mass etc., when you're pretty sure to get inertial effects. If these aren't present, or not important to you, you could just analyse it in a couple of steps statically using implicit.
Secondly, the analysis time using explicit time integration is proportional to the smallest element size in the model - the smaller the element, the smaller the time step, the longer the analysis takes etc. (this is based on the speed of wave propagation across the elements of your model). So try and keep your mesh as uniform as possible to avoid this, and go to a more coarse mesh if you can.
Cheers,
-- drej --