Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here


Blast Design in FEA - what acceptance criteria

Blast Design in FEA - what acceptance criteria

Blast Design in FEA - what acceptance criteria

Hi All,

My question is in regards to blast design in FEA, e.g. using ANSYS Explicit Module.
I will create steel structural system consisting of shell/plate elements only, this means any girders will be simulated by few shells.
Loading will be transient with peak value simulating the blast.

Please let me know, against which code and allowable criteria would you check stress results values (for shell/plate elements from FEA) to satisfy any blast code requirements?

RE: Blast Design in FEA - what acceptance criteria

Hi again

Im waiting for my LS-DYNA explict run to followup.

In blast engineering you expect elasto-plastic response, so generate elasto-plastic material curves for steel. Its not about stress so much as it is about for deformation.

Since blast engineering is all about ductility, you want to measure/look at strain and make sure it isn't past the ultimate tensile strain of the material (rupture). In short look at effective plastic strain and compare to maximum allowable plastic strain of material.

Good primer on blast engineering is the US's Unified Facilities Code for blast engineering, has some hand examples and concepts.

Hope this helps

Pipe Stress Analysis Engineer

RE: Blast Design in FEA - what acceptance criteria

Jeff, once more, thanks for helping me in two parallel threads, which are related to each other! Much appreciated.
Figures you have attached are clearly describing the example.

I have one question
, lets please focus at plastic strain plot of yours. Let's assume 1.5e-02 is the max allowable value given in the code. Plot is a snapshot from the 0.075 time range, as such we know that earlier in time some smaller areas of your structure started to be red of strain values 1.5e-02. The question is how do you know how long / to what extent you may allow red areas to extend over your structure? Perhaps you are measuring also some angular deformation to be less than 2 degrees, or more probably you have some additional information from the code what length of the area with red values (1.5e-02) is allowed?

RE: Blast Design in FEA - what acceptance criteria

JGard1985 , I will much appreciate your response on the question above.

RE: Blast Design in FEA - what acceptance criteria

Glad to help.

In the picture you're refering to I clipped the contour plot of effective plastic strain (EPS) at 1.5E-02 (to get a nice looking plot). So basically I set the contours for the fringe plot. One locally stressed element had an EPS of 0.18, so my cropping of the contour limits makes the figure "look pretty" for the customer. It shows highly stressed regions in the framing members. We really weren't concerned with local yielding at corners of windows and doors. Also I don't remember if this was the final design (satisfactory?)

Regarding your question, your analysis needs to be strain dependent. For your analysis, determine maximum allowable strain and corresponding EPS. This is a function of material properties (Percent Elongation)

Then compare your FEA predicted strains and EPS against the maximum allowable strain.

Duration of the ductile response really isn't a factor as long as you have captured the maximum displacement of the structure (look for a rebound).

You can also check rotation but, I prefer to do this by taking some manual measurements and doing a little trigonometry.


Pipe Stress Analysis Engineer

RE: Blast Design in FEA - what acceptance criteria

Thanks Jeff!
Am I right to say that your EPS value of 1.5E-02 (as per example) was lower than maximum allowable strain?
I thought EPS value was equal to maximum allowable strain, that is why I have asked what area size of the max utilized strain value is within the limits.

RE: Blast Design in FEA - what acceptance criteria

Yes my upper bound fringe plot threshold 1.5E-02 is lower than maximum allowable strain. Depending upon material your maximum allowable strain could be in range of 0.22 to 0.3. EPS is calculated from FEA and needs to be less thn allowable strain

Can you clarify what you meant by: I have asked what area size of the max utilized strain value is within the limits.


Pipe Stress Analysis Engineer

RE: Blast Design in FEA - what acceptance criteria

Certainly, the best will be to cite DNV non-linear code as this is not something I have invented, rather that is code clause which is based on experience and laboratory tests:

The strain limit for gross yielding reflects that real structures will include elements of inhomogeneity that
will not be accurately modelled in the analyses. This will mean that the strain measured over a long length
of a real structure will in average not reach the values that can be found in standardized tensile tests.
With gross yielding is meant that plastic deformations with strain above 2% are taking place over a zone
lyz > 20t in the direction of the maximum plastic strain.
The maximum gross yielding strain in any integration point, in any element within the yield zone, should
be limited to the gross yielding critical strain.

RE: Blast Design in FEA - what acceptance criteria

Oh I see where you went, DNVGL-RP-C208, right?

I don't design in accordance with this code (mostly design in accordance with US Army Corps of Engineers facilities design criteria and AISC).

Its pretty common in blast engineering to expect large gross yielding, so I haven't really checked against this requirement in DNVGL-RP-C208. I avoid irregular geometry (bolt holes) in my flexural members that could produce localized yielding or failure. I do check against an upper bound limit state (EPS) and ductility limits prescribed by the respective code.

Pipe Stress Analysis Engineer

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members! Already a Member? Login


eBook - Rethink Your PLM
A lot has changed since the 90s. You don't surf the Web using dial-up anymore, so why are you still using a legacy PLM solution that's blocking your ability to innovate? To develop and launch products today, you need a flexible, cloud-based PLM, not a solution that's stuck in the past. Download Now
White Paper - Using Virtualization for IVI and AUTOSAR Consolidation on an ECU
Current approaches used to tackle the complexities of a vehicle’s electrical and electronics (E/E) architecture are both cost prohibitive and lacking in performance. Utilizing virtualization in automotive software architecture provides a better approach. This can be achieved by encapsulating different heterogeneous automotive platforms inside virtual machines running on the same hardware. Download Now

Close Box

Join Eng-Tips® Today!

Join your peers on the Internet's largest technical engineering professional community.
It's easy to join and it's free.

Here's Why Members Love Eng-Tips Forums:

Register now while it's still free!

Already a member? Close this window and log in.

Join Us             Close