News: HyperSizer.com has a Community Board and Customer Support System. Submit a ticket at http://hypersizer.com/ticket

Author Topic: FEA loads procesing for DSP  (Read 1094 times)

David Hughes

  • Client
  • **
  • Posts: 3
    •  
FEA loads procesing for DSP
« on: February 20, 2020, 07:53:31 AM »
Hi,

I am trying to follow how HyperSizer is calculating the Discrete Stiffened Panel loads for technique 2 so as I can understand the limitations. Apologies for the long message, but I have a few questions:

1) When creating the segments there is an option to create a stringer or frame segment. What’s the difference?

2) After upgrading to v8.0.47 I noticed that there is a new DSM backdoor option:
"Modify technique 2 beam fea moments to account for stiffener height"
What does this mean? Is it something related to bar offsets, or is it the moment correction for Cruciform sections, or is it something else?

3) V8 now incorporates the integral cruciform concept into the native environment, however there is no specific documentation. Is it the same as the method/equations used for the Metal Grid Stiffened Plugin?

4) Within the FEA Loads tab why are the tension and compression tables empty?

5) Within the FEA Loads document, section 4 gives the equations for the N-sigma methods. Do similar equations apply for BAR elements using length instead of area? Also, I cannot match the standard deviation values. Is the equation missing an n term (where n=number of elems) or is it something else?
   SD = (Sum((Ni - Navg)^2*Ai)/(((n-1)/n)*Sum(Ai)))^0.5

6) Within the FEA Loads document for Discretely Stiffened Panels I believe the transformation equations are incorrect (eq. 1 to 3):
   Nxy = -Fx*cos(q)*sin(q) + Fy*cos(q)*sin(q) + Fxy(cos^2(q)-sin^2(q))
   Similar for Mxy
   Qxx = +Vx*cos(q)+Vy*sin(q)
   Qyy = -Vx*sin(q)+Vy*cos(q)

7) For the Discretely Stiffened Panel’s transverse shear summation (eq. 41), I’ve found cases when the skin load relieves the total. I haven’t noticed this for Nx,seg and I’m still working on Mx,seg. I believe the full Qx,seq equation is:
   Qx,seg = (V1 + sign(V1)*(Qxx,L*wL/2+Qxx,R*wR/2)))/(1/2*(wL+wR))
   Where:   V1 = if |V1,t|>|V1,c| then V1,t else V1,c
   Similarly for Qxx,L and Qxx,R
Test case;
   wL/2 = 100   wR/2 = 100
   Qxx,t,L = 0.5   Qxx,t,R = 6.0
   Qxx,c,L = -1.0   Qxx,c,R = -3.0
   V1,t = 200   
   V1,c = -500   
      
   V1 = -500
   Qxx,L = -1.0
   Qxx,R = 6.0

   Qx,seg = (-500 - (-1.0*100 + 6.0*100))/200 = (-500+100-600)/200 = -5N/mm
Note that the LH Skin is relieving the load.

Kind Regards,
David
« Last Edit: February 20, 2020, 08:01:08 AM by David Hughes »

David Hughes

  • Client
  • **
  • Posts: 3
    •  
Re: FEA loads procesing for DSP
« Reply #1 on: February 21, 2020, 10:34:30 AM »
Hello again,

Is there a failure mode that uses Qx,seg? If not, please ignore question 7 in my previous message.

I'm struggling to calculate Mxx,seg with N-sigma method and the tension/compression loops. Could you please explain the calculation process?

Also, the DSP loads document (sect 3.4) states that the smeared ABD method is used to calculated object forces, whereas the grid stiffened plugin had a different set of equations for the reference stresses. What does v8 use now for the integral blade and cruciform concepts? How are the tension/compression loops fed into these calculations?

Regards,
David.

Brent

  • Administrator
  • *****
  • Posts: 23
    •  
Re: FEA loads procesing for DSP
« Reply #2 on: March 11, 2020, 04:19:21 PM »
Hi David,

Answers numbered below:

  • Behind the scenes, they are exactly the same. The only feature that uses the different names are the 2D maps.
  • This flag is obsolete and is now the default behavior. Unfortunately we did not remove it from the interface. We will include the update on the next release. A little background, originally the segment bending moment contribution from the bar elements was only M1 or M2. This flag would allow the axial component of load in the bar element to contribute to the segment bending moment due to the shift in the neutral axis of the bar to the mid-plane of the skin. The later is now the default behavior. Sorry for the confusion.
  • The documentation is in work right now. Additionally, we will have an update to the Grid Stiffened Plugin to support the discrete cruciform component concept. There are some difference in the section properties calculations between the Grid Stiffened Plugin and the HyperSizer native approach.
  • Unfortunately HyperSizer does not report the tension and compression tables on the FEA Load Tab for discretely stiffened panels. The attached image shows some additional reporting that is accessible from the sizing form after analyzing a single component. These files have some tension and compression load details that you might find useful.
  • Correct, bar elements use the following equation for the tension and compression loops:
    Pavg + N*Sqrt(Sum(Px,e-Pavg)^2*Le/Sum(Le)), where "e" denotes element and L is length.
    Or more simply put for 0-sigma:
    Sum(Px,e*Le)/Sum(Le).
  • Good Catch! The documentation was incorrect for the equations you noted. See attached image for updated transformation equations 1 through 3. We'll update the documentation
  • Looking at the example provided. I noticed that you are combining a tension load state in the right skin with a compression load state in the stringer and left skin. Are you saying this is the behavior reported in HyperSizer?
  • Qx,seg is used in the calculation of the stringer shear load. You can verify this by switching between segment loads and object loads in the backdoor options.
  • HyperSizer v8 native criteria uses the ABD approach for computing the object loads.Regarding your question about tension/compression loops, are you asking about how are these loads fed into the plugin calculations or the HyperSizer native criteria calculations?

Lastly, can you provide the specific example you are struggling with?

-Brent