SYSTEM UNITS

[ENCHTAIN]

hi everybody,

How i can know the system units used by ansys, and how can i change them without using commands.

thanks a lot.

 

[Lirock]

Hi,
There is no fixed units in ANSYS. It's just depends on you. If you make the geometry model dimension with meter, then the material properties and other datas should be defined with meter; if you use millimeter, then the other datas must be defined with millimeter.
I don't know whether I make it clear. Hope to help.
Regards!

Rock Li

 

[ENCHTAIN]

Hi,
thank you for your reply, but for example, if i want to create a line by 2 keypoints, these keypoints will be created with there coordinates without specifying the unit (exemple:first keypoint(0X,0Y,0Z) second keypoint(10X,0Y,0Z), so the length of the line will be 10.the problem is that 10 has no meant without its unit???

 

[cbrn]

Hi,
"10 has no meant without its unit": --> that's the point. YOU give this value the meaning YOU want. It can be 10 microns, 10 millimeters, 10 meters, 10 light-years. The important thing is to apply dimensional analysis and find out the reciprocal scale factors between the foundamental units and the derived ones. This can be tricky, sometimes. For example, in a system where length is in mm, time is in seconds, force is in Newton, then the pressure is in MPa and this is obvious, but mass is in tons and this is less obvious at first sight...

Regards

 

[aphilic]

Hi,

You can not specify any unit into Ansys and you do not have to. In your example, you have to see it 10 Units and thats all. I mean it can be either 10 kilometer (if you accept 1 Unit = 1 kilometer) or 0,5 milimeter (if you accept 1 Unit = 0.05 milimeter) and it does not matter at all. It is up to you. However, you must pay attention whatever unit you use, you must use the same unit for the rest values you enter. All other materal properties, forces, displacements and anything related to that unit you use, must be defined as the same unit.

Hope this helps.

Regards,

Can

 

[aphilic]

Oups, sorry cbrn, i didnt see your post. I didnt mean to send over yours. Sorry again...

 

[ducking]

ANSYS uses for defect the MKS system (always), therefore, your 10 will become 10 meters,
For example in electromagnetics (my area)if you want to change this system use:

Preprocessor>MAterial Props>Electromag Units



Lucky
ducking79@hotmail.com

 

[cbrn]

Hi,
ducking, foundamentally incorrect. Ansys provides some sets of correlation factors in particular sub-branches (e.g. EMUNIT, PUNIT, EXUNIT), but they are not meant to physically represent true dimensions. Cited from the manual, from the explanation of "/UNITS" command:
"The units label and conversion factors on this command are for user convenience only and have no effect on the analysis or data".
There is no such thing as a "default" for the system of units used in the user's "simulation world". It's the user which must ensure he inputs the values in a consistent system.
The "default to MKS" you say is a mere coincidence: it must be thought as having all the conversion parameters set to 1 (unity). Obviously, if your solid model is also made in "m" (in the CAD, for example), you will have a "pseudo-true", automatically-set, MKS system. But once again, it's a coincidence, or better said a user-convenience. Let's take an example:
Let's consider a cube in arbitrary dimensions 2x2x2. You can leave all the conversion parameters to 1 (so you would say that Ansys is working in "MKS"), but now, what would say that your cube has a volume of 8 cubic-METERS? Ansys? Surely not!!! If, despite the "MKS" setting in the /UNITS, I now input a material density of 7.85E-9, I'm free to "think" my model as being in a "MPA" world, with mass expressed in tons (not kg as the "MKS" setting would say), thus having a mass of 62.8 milligrams, and with pressures in MPa (and not Pa). I'll then input a gravity of 9810 (thinking it as "mm/s^2"), and so on. But I could also be in a black-hole, then 9810 would be in "m/s^2" and my material would be some kind of very rarefied gas, and my cube would be in "m"... All this, without touching the "/UNITS,MKS" setting !
The "units" in Ansys are merely labels. It's totally different from other FE packages (mainly those which work embedded in CAD systems, for obvious reasons), where you can see that choosing a unit-system DOES HAVE an effect on the analysis (in fact, for example, by changing the unit-system a conversion is made in the values of loads, imposed displacements, etc...).
Note that, as Drej said in another discussion on the same topic, in reality FEM doesn't have the concept of "units": when other packages let you choose a "unit-system", in fact they "force" you to choose among some pre-defined sets of internal conversion parameters: being these factors known from the start, the programmers have built-in routines to perform the conversions "on the fly". But once again, all this is really useful only when the FEM is directly linked to another "world" (CAD) where the length-unit choice is mandatory.

Enchtain, the /UNITS command can not be accessed by menu.

Regards

 

[jorand]

Ansys use the command /units
USER — User-defined system (default).
SI — International system (SI or MKS; m, kg, s, K).
CGS — CGS system (cm, g, s, °C).
MPA — MPA system (mm, Mg, s, °C).
BFT — British system using feet (ft, slug, s, °F).
BIN — British system using inches (in, lbm, s, °F).

if I want use the unit BFT then all my parameter how permitivity, resistivity, temperature, are in BFT

 

[ducking]

Hi
cbrn, I have to admit that you are correct, I just can say from your exaples, as you said, "It's the user which must ensure he inputs the values in a consistent system"

Regards
Lucky