units

[andrearrd]

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

 

[corus]

yes, consistent units are N/mm^2

corus

 

[Drej]

Andreard,

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 --

 

[andrearrd]

thank you all for your prompt replies. Drej, would density not be input in tonnes/mm^3 so as to keep the Newton cosnistent, beacsue F = m a and if acceleration is in mm/s^2 then mass should be in tonnes?

 

[Drej]

If you're using Tonnes (metric), then you should definitely use m/s^2 as your acceleration unit since:

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.

 

[andrearrd]

thank you drej but i am still really confused! I am suing mm in my parts, and want to use Newtons as my force. Then do i input density in kg/mm^3 or tonne/mm^3? 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 . 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

 

[Drej]

What haven't I made clear? What is your definition of a Newton force?

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.

 

[corus]

The density is irrelevant for a static analyis. For a dynamic analysis Abaqus recommend tonnes/mm^3 if you're using mm and Newtons and your acceleration in mm/s^2, velocity in mm/s. For a thermal analysis you have to use kg/mm^3 as specific heat is in J/kg C (usually), just to confuse things.

corus

 

[andrearrd]

hello.
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

 

[Drej]

Having sat down in a dark room for a while thinking about this (and actually WRITING the units down), you can do it several ways. However, you're correct in the use of T/mm^3 and mm/s^2 (my apologies), as this will give you your N unit. The first method I mentioned is also consistent. As pointed out by corus, if this usage (Tonnes and mm/s^2) is recommended by ABAQUS then, of course, run with it.

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 --

 

[andrearrd]

ok tahnks drej. on another note, im doing an explicit analysis. A stiff material is expanding onto a very soft material (via a pressure applied on the stiffer material), and i get very undesirable inertial effects i think because of the loading rate. However adding more steps to make the laoding more gradual just results in everything taking ages. is there a way of somehow slowing things down?

thanks again

 

[Drej]

I don't fully understand what you're trying to do, but I've got a few suggestions. Apologies if I'm teaching you to suck eggs here.

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 --