ANSYS - prestressed column with increasing load 1

[HStruct]

Dear FEA gurus,

I am wondering if somebody can help me with this situation.

1. I have a column (with 1000x1000x2000 units dimentions) compressed by a load of 100 units.
2. After the solution is done in ANSYS I want to keep the column in compression (prestressed) and add another compressive load of say 100 units.

It seems pretty simple but the the column is not holding the stresses due to first loading during second loading. I have tried Prestres option however doesnt seem to work.

Could anybody please suggest me how to do it?

-HMT

 

[jiligeo]

Dear HMT, did you try to save the stress results in a file and act it again on the structure as initial stress?
you can use the following commands:

iswrite,on
.
.
.
isfile,read,,,,0

 

[HStruct]

Thanks A Lot Jalil,

I had been busy with another problem. I just read all about it (iswrite and isfile)from ANSYS, I will try it out, hope it works for me.

-HMT

 

[jiligeo]

Dear HTM, maybe you can solve your problem easier.
If you leave the solution for checking the results after first load step, you have to choose restart option (solution>analysis type>restart) and in “Action” choose “continue”.

Hope to help you

 

[JacobL]

I'm from a NASTRAN background, but this seems like a non-linear solution, with non-linear material behaviour.
Your material is probably nearing the limit of elasticity on the initial loading, with high displacement, and then you want to go over to the plastic strain with higher displacements.

As to HOW to do it in ansys, haven't a clue, but the methodology should be generally the same.

Jake.

 

[Lirock]

There maybe no limit of elasticity defined in ANSYS, so even the stress went over it, the model will still present as a elasticity one

 

[HStruct]

Hey Liweisc,

That is correct, it was just a sample model for my original model, thus I didnt define any elasticity limits and I wanted my model to be only in elastic range.

I cant use "iswrite" or "isfile" because I have shell63 and contact elements in my original problem and these two commands don't support shell63 and contact elements, thus "iswrite" doesnt write initial stresses for these elements.

I'm not able to use "RESTART" either because after my 1st load step I need to build my model in size which creates more elements addition to the old ones and ".esav" contains only the old elements. WHen I retsart the SOLUTION, ANSYS gives an error "number of elements in .esav not same"

Anybody knows how to handle this situation? Please help ..

Thanks,
-HMT

 

[jiligeo]

Dear HMT, just a comment on using the contact elements. I have also in my model contact element with initial stress. You have to unselect all contact and target elements before defining the initial stress.

/solu
esel,u,type, ,2
esel,u,type, ,3

isfile,read,,,,0

Regards
Jalil

 

[amini06]

Dear HMT

Thanks for your comment about my Q,"Applying Initial Condition but non-cumulative results".

I used istr. command for a test example:
In this Examp,First I used a cncentrate load,say F,on a node & wrote the stress results on a file(ISTR.IST)by using ISWRITE,on after f command.
Then the Examp. rewrote by ignoring F effect & using stresses values file by: ISFILE,READ,ISTR,IST,,1 .(Based on ANSYS Help Commands)
But I saw an amazing results,stresses are not transfer logically from integration point to nodes,the values are very very smalls,also the deformed shape is completely inverse!!


May I have your idea?

Regards

 

[HStruct]

Hey Amini,

You have noticed a very good point here, about the inverse deflection shape of the cantilevel. I also have thought about it, and in fact I have done a little bit of research for that INVERSE DEFORMED SHAPE.

This is what I conclude - the ISWRITE writes the stresses which will surely be oposite of what you would think generally.

Thus say you want a deflection (from that example) of -0.796 Units, you will have to
1. apply a force of 1E5 units to create ist file by iswrite.
2. then read that .ist file in another program using isfile with additional load of -1E5 units.

Interesting huh?

Well thanks for sharing your idea....
-Hemant

 

[cbrn]

Hi,
I never tried it so I won't be able to help you, but the general idea when two successive loadsteps have to have different number of elements is to use "element birth / death".

Regards