Request for help with Analysis and Constraints

About the development of the FEM module/workbench.

Moderator: bernd

Laurie Hartley
Posts: 522
Joined: Mon Feb 27, 2017 5:33 am
Location: Australia

Request for help with Analysis and Constraints

Post by Laurie Hartley »

I am trying to simulate a situation that I will try to describe:-

I have a CHS with a polar array of four pockets 16mmxby 62.5mm long
The top of each pocket is 95mm from the top "end"face of the CHS
I want to apply a force of 6472kn to the top "end" face of the CHS
Inserted in each pocket is a steel member of exactly the same dimensions as the pockets.
For the sake of this exercise the steel members cannot move in any direction.
I would like to establish what forces the corners of top faces of the pockets are able to resist before they "crack" ,

I have the force constraint on the top end face of the CHS and a fixed constraint to the top faces of the pockets but I can't figure out if I need to add any displacements to the sides of the pockets.

Any help will be appreciated

I tried to do this using a face binder but I got a strange result so I went with the actual part and a netgen mesh.
I have attached the file and an image of the face binder
Attachments
Converter Tube - 48.3.FCStd
(38.54 KiB) Downloaded 45 times
distorted shapebinder.png
distorted shapebinder.png (29.82 KiB) Viewed 2016 times
User avatar
NewJoker
Veteran
Posts: 3021
Joined: Sun Oct 11, 2020 7:49 pm

Re: Request for help with Analysis and Constraints

Post by NewJoker »

Those bricks in the pockets are excluded from the mesh. If you want to include them in the numerical model, you should make a union or compound of all parts. Then you will be able to apply boundary conditions also to the bricks. Otherwise, constraints applied to them won't be accounted for.

Of course, the whole scheme of constraints depends on how the structure is supported and loaded in real life. Maybe you could start by fixing the outer faces of the bricks once they are meshed with the rest.
Laurie Hartley
Posts: 522
Joined: Mon Feb 27, 2017 5:33 am
Location: Australia

Re: Request for help with Analysis and Constraints

Post by Laurie Hartley »

NewJoker wrote: Mon Sep 12, 2022 9:27 am Those bricks in the pockets are excluded from the mesh. If you want to include them in the numerical model, you should make a union or compound of all parts. Then you will be able to apply boundary conditions also to the bricks. Otherwise, constraints applied to them won't be accounted for.

Of course, the whole scheme of constraints depends on how the structure is supported and loaded in real life. Maybe you could start by fixing the outer faces of the bricks once they are meshed with the rest.
Thanks NewJoker for your response. I left the “bricks” out of the mesh deliberately to try to keep things simple* but they are part of what is going to resist the CHS “going to ground”. I included them in an attempt to show what the connection would be (no welds just contact).
*Doesn’t always work for me :D

Putting it another way the force will stop at the top of the pockets but can keep travelling down the areas between each pocket creating what I think is a shear stress.
thschrader
Veteran
Posts: 3129
Joined: Sat May 20, 2017 12:06 pm
Location: Germany

Re: Request for help with Analysis and Constraints

Post by thschrader »

Here is a contact analysis using a 1/4 model (and 1/4 force).
GMSH: use first order elements
The brick is xyz-fixed at the bottom, contact surface is top of brick/top of opening.
Stresses arent high...
ConverterTube483.FCStd
(69.98 KiB) Downloaded 42 times
Laurie Hartley
Posts: 522
Joined: Mon Feb 27, 2017 5:33 am
Location: Australia

Re: Request for help with Analysis and Constraints

Post by Laurie Hartley »

thschrader wrote: Mon Sep 12, 2022 11:54 am Here is a contact analysis using a 1/4 model (and 1/4 force).
Getting late here Thomas but I am looking forward to examining your file tomorrow.
Laurie Hartley
Posts: 522
Joined: Mon Feb 27, 2017 5:33 am
Location: Australia

Re: Request for help with Analysis and Constraints

Post by Laurie Hartley »

@thschrader I downloaded your file and examined the boundary conditions Thomas - that is what I was trying to do (rather clumsil I must say). To me looking at your file is a thing of beauty and I have taken on board that it is good practice to break models down into smaller components if possible.

This business of contact analysis is very complex is it not? but also very important in my understanding.

I opened the file and hit a snag though - see note below and image.
NOTE - at end of calculix output.

Number of contact spring elements=0
Using up to 8 cpu(s) for the stress calculation.
Using up to 8 cpu(s) for the symmetric stiffness/mass contributions.
Factoring the system of equations using the symmetric spooles solver
Using up to 8 cpu(s) for spooles.
Using up to 8 cpu(s) for the stress calculation.
average force= 574505134.495308
time avg. forc= 574505134.495308
largest residual force= 7048479803080.648438 in node 12643 and dof 3
largest increment of disp= 4.454344e+08
largest correction to disp= 3.848437e+08 in node 6662 and dof 3
divergence allowed: residual force too large
divergence allowed: number of contact elements stabilized
divergence; the increment size is decreased to 9.765625e-04
the increment is reattempted
reducing the constant stiffnesses by a factor of 100
*ERROR: too many cutbacks
best solution and residuals are in the frd file
78.5: CalculiX execute error:
78.6: Loading result sets...
Attachments
Gmsh setup.png
Gmsh setup.png (172.1 KiB) Viewed 1851 times
Laurie Hartley
Posts: 522
Joined: Mon Feb 27, 2017 5:33 am
Location: Australia

Re: Request for help with Analysis and Constraints

Post by Laurie Hartley »

I opened it and ran gmsh and calculix again without any problem - I don't think I did anything differently.
Below is a screenshot of the TRESCA stress. Does that look correct?

This is the content of the ccx_dat_file:-

total force (fx,fy,fz) for set CONSTRAINTDISPLACEMENT and time 0.1000000E+01

3.063001E+00 3.063291E+00 -1.617888E+03

total force (fx,fy,fz) for set CONSTRAINTDISPLACEMENT001 and time 0.1000000E+01

-3.063001E+00 -3.063291E+00 4.678447E-13

total force (fx,fy,fz) for set CONSTRAINTDISPLACEMENT002 and time 0.1000000E+01

3.641532E-14 -4.440892E-15 1.617888E+03
Attachments
ksnip_20220913-171456.png
ksnip_20220913-171456.png (219.43 KiB) Viewed 1806 times
thschrader
Veteran
Posts: 3129
Joined: Sat May 20, 2017 12:06 pm
Location: Germany

Re: Request for help with Analysis and Constraints

Post by thschrader »

Laurie Hartley wrote: Tue Sep 13, 2022 2:35 am ...
This business of contact analysis is very complex is it not?
...
Yes, and I am not very good at it. I dont need contact
analysis for my daily work. The calculation was done to get a first
impression how the stresses could look like.

However, lets run a "normal" analysis.
I slightly reduced the brick dimensions, mesh connection only on top,
the red line. A classic hand calculation would give 40 kN max loading on
the tube, including a safety-factor of 1,5. When running the linear-elastic FEM (default),
you get excessive stresses in the corners, peak up to 1800 MPa. This is far too high.
Conclusion when using max stress as criterion: max load must be reduced
But is that true?
Lets use the critical-strain criterion as described here:
https://forum.freecadweb.org/viewtopic.php?f=18&t=35893

Running the plastic analysis and using the yield-curve for S235 as described in the
DNV-manual, you get a peak stress of 300 MPa (much better) and a
equivalent plastic strain below 2%. Acceptable is 5%.
Conclusion: 40 kN loading is ok. Stablity/buckling not checked...

Be patient, when re-running the file, ccx needs 500 sec.
ConverterTubeStresses.FCStd
(62.8 KiB) Downloaded 40 times
elastic_vs_plastic.JPG
elastic_vs_plastic.JPG (126.2 KiB) Viewed 1776 times
Laurie Hartley
Posts: 522
Joined: Mon Feb 27, 2017 5:33 am
Location: Australia

Re: Request for help with Analysis and Constraints

Post by Laurie Hartley »

@thschrader Thanks Thomas - more to study and learn over the next couple of days. I had been looking at the link already. I already have at least two questions in mind.

Just one thing I want to “own up to” - in my OP I stated a load of 6472kn - enough to send an engineer running and screaming down the street :shock: I meant of course 6.472kn (or 660kg) - I missed the decimal point after the 6 out. :oops:
Laurie Hartley
Posts: 522
Joined: Mon Feb 27, 2017 5:33 am
Location: Australia

Re: Request for help with Analysis and Constraints

Post by Laurie Hartley »

Laurie Hartley wrote: Tue Sep 13, 2022 11:27 am @thschrader Thanks Thomas - more to study and learn over the next couple of days. I had been looking at the link already. I already have at least two questions in mind.
I spent the last couple of weeks trying to get a better understanding of this topic. I read the links(s) by HarryvL - I found that quite challenging but I took on board his comments and yours about the way FEM sort of punishes us with stress results.
Nevertheless I didn't like the look of those "hot-spots" in the top corners of the tube pockets and felt I could alleviate them by introducing curves into the pocket corners and chamfers to the top edges of the brick.

So I have attempted to produce a new model along those lines. I am am not sure whether it is a viable model but it seems to work.
I tried to follow the design principles and constraints in your file and after watching this youtube video by Danial Iskhakov
https://youtu.be/HINdN0wW1d0

The one area I struggled with was introducing the mesh regions _ I just couldn't figure out how to get them into the analysis tree??

I increased the force to 40kn/4 = 10kn and as you suggested despite the smaller contact area (I like your equation :D ) things look pretty good.

I have attached a link to my file:
https://www.dropbox.com/s/0d5pq5sb0p59w ... FCStd?dl=0
Post Reply