Hi Dear

do following Stage respectively:

1-you must  have 2 Files(.cae) :1-1-Static Analysis 1-2-Explicit Analysis

2-in first File you have only Static Step and apply Gravity Load then Run it

3-Save Jop file for Static File and remember its name and 

4-Create Explicit File(Explicit Analysis)"a new file with previous model" .  in Load Step :

4-1-go to predefined Field manager and select initial Step then  select Stress

5-so select  all model and Select (Specification : from output file)

6-so select Static File(Stage 3)

Best Regards

Alireza 

Dear Dileep Mani,

As far as I know, you will have to apply your gravity load in a preliminary step using a time period which is long enough so as to not induce a dynamic response.

Hope this helps.

Best regards,

Mahir

Hi Dear Dileep Mani,

you must first define gravity load in Static Step  next  apply (gravity load) as  predefined Load  in Explicit Step

Best Regards

Hi alireza, 

I gave gravity load in static general step. But after that step I can't select dynamic explicit. Can you kindly explain it.

Greetings..

Hi Dear

do following Stage respectively:

1-you must  have 2 Files(.cae) :1-1-Static Analysis 1-2-Explicit Analysis

2-in first File you have only Static Step and apply Gravity Load then Run it

3-Save Jop file for Static File and remember its name and 

4-Create Explicit File(Explicit Analysis)"a new file with previous model" .  in Load Step :

4-1-go to predefined Field manager and select initial Step then  select Stress

5-so select  all model and Select (Specification : from output file)

6-so select Static File(Stage 3)

Best Regards

Alireza 

@Alireza

This is very interesting. I am using ABAQUS 6.10. There, I am not given the option "Stress" if I follow your instructions.

Which version of ABAQUS do you use?

Best regards,

Mahir

Hi Dear Mahir Ülker-Kaustell 

Thanks , i use ABAQUS-V6.12

V6.10 don't have this item

Best Regards

Alireza

@Alireza

No, it is I who thank you. This can become very helpful för me, those preliminary steps have been quite annoying in the past. But now, if I need the explicit solver, that problem is fixed.

Thank you.

Best regards,

Mahir

 Hi alireza,

I did as you explained and it is working perfectly.

thank you very much.

Greetings..

How the mass scaling is done for Dynamic Explicit.

Thanks....Also when I am trying to do Explicit Analysis after Static as per the procedure given above. It is asking me:

Specification : From output database file  ( I am selecting this)

File name: Here I am selecting the odb file of Static analysis.

Step: Here I could not type anything or select

Increment : Here also I could not type anything or select

And lastly I am getting an error data is not complete.

Can you please help me in this regard.

Thanks

I was trying a similar simulation. I faced a different issue.

During explicit analysis, the predefined stress are relaxed and naturalized.

Hi,

After applying gravity load in a dynamic explicit step, the analysis runs successfully. Kinetic energy is a very small fraction of internal energy of the model. What kind of deformations I should expect? Should they be negligible? For example, in geostatic step, usually negligible deformations are obtained. Does this analysis should also produce negligible deformations? Thanks.

Hi,

I wan to perform a cyclic analysis (on a steel brace) with gravity load (brace's self-weight) included. (Dynamic Explicit).

I want to preload the brace with its self-weight, gravity load (STEP 1);

then keep the gravity load active and apply the cyclic loading (STEP 2).

The question is:

Is the effect of the gravity load still being active during the cyclic loading? Not just as an initial condition for the STEP 2.

The PROPAGATED option for the gravity load will assure this phenomenon?

Gravity load can not vary during the whole analysis.

I had the same problem. I tried to apply gravity load in a dynamic explicit step by means of smooth step, but this introduced much kinematic behavior because of the variable velocity of smooth definition. I recommend to use "tabular step" by entering an amplitude ramp definition (i.e. Time: 0,0.1 and Amplitude: 0,1). It should work better. However, I also recommend to give the general dynamic explicit step a little more time than the amplitude definition "tabular step" (i.e. Time step 0.2). This is to achieve a steady state of gravity load application before applying any additional load to the structure.