Strand7 geometry 1

[eqgeotech]

Need to clean geometry and plate free edges, I am not able to connect/attach plate free edges. I am attaching a pic of the model, "yellow" outlines are plate free edges. please help

 

[HawksOkeyoJr]

Which software are you using to clean the Geometry??. Can you attach the model too or it's too big?, with that, we can be on the same page as we try to solve the issue.

 

[IDS]

Tools-Clean-Mesh will join all compatible elements.

You know that plate elements can only join at an edge if they have the same corner nodes (and mid-side nodes, if they have them)? You can't join two or more short edges to a single edge of a bigger element.

Have you downloaded the new manual?

Doug Jenkins
Interactive Design Services

http://newtonexcelbach.wordpress.com/

 

[eqgeotech]

Thank you IDS hope it works

 

[jhardy1]

It looks like you have gone from a relatively coarse mesh to a fine mesh in places, meaning that you are attempting to join multiple element edges on the "fine" side to a single element edge on the "coarse" side. You need to use "grading" over several element widths to transition from a fine mesh to a coarse mesh, to ensure compatibility at all adjoining element edges.

http://julianh72.blogspot.com

 

[eqgeotech]

jhardy1: here I need to connect plate (soil) element with beam element, I need to connect the plate free edges, how can I use grading for cleaning plate free edges on inner side.

 

[eqgeotech]

IDS: Can you please tell me which link should I use to connect nodes at the corners of plate (soil) element (in pink colour) to connect to beam elements.

 

[jhardy1]

I assume you have a mesh that has incompatible element edges - something like the attached "Incompatible Mesh" screen shot.

You need to do something to match the number of nodes across the incompatible junctions. E.g. use the "Grade Plates and Bricks" tool, and select a row of elements on the "coarse" side of the junction (see "Selected Elements"). This will subdivide the selected elements (according to which "Grade" tool you have chosen), to produce a compatible mesh similar to the attached "Graded Elements". It's not a pretty mesh, but at least it is node-compatible.

You could then try using the "Smooth Plates" tool to generate a smoother graded mesh (similar to "Smoothed Elements") - still not an ideal mesh, but it's heading in the right direction.

Hope this helps!

http://julianh72.blogspot.com

 

[eqgeotech]

Thank you jhardy1 and IDS , some of the problems are fixed, now I need to apply earthquake time history and determine the site response for the current structure, can u help me with that.

 

[eqgeotech]

I am using rayleigh damping in my case and have both the frequencies w1 and w2 but i dnt know how to find the corresponding damping ratios.

 

[IDS]

IDS: Can you please tell me which link should I use to connect nodes at the corners of plate (soil) element (in pink colour) to connect to beam elements.

There are several options:
1 Rigid links; select Create-Link and choose rigid from the drop down box
2 Create a beam type with properties of concrete and appropriate cross section area, but zero mass so you don't double count the mass
3 Create a beam with "point contact" properties, which will transfer compressive normal forces and friction forces limited by the friction factor

I'd suggest trying 1 or 2 to get the model running. You might look at 3 if you get a large shear transfer across the base of the footings, but this will need a non-linear analysis which will make things much more difficult with a time history analysis (and there isn't much point unless you are using a non-linear model for the soil and concrete as well).

For appropriate damping refer to standard textbooks and try a range of values.

Doug Jenkins
Interactive Design Services

http://newtonexcelbach.wordpress.com/

 

[jhardy1]

"now I need to apply earthquake time history and determine the site response for the current structure, can u help me with that."

With respect, it sounds like you need a LOT of assistance / mentoring to get up to speed with the task that you have been assigned. (Is this a student posting?) What you are asking is a bit beyond the scope of a forum such as this to provide useful support.

You should read some FEA reference texts, and check out the Strand7 Reference Manual and Verification Manual (which should be installed on your C: drive in the program folder). Also, assuming you are a supported Strand7 user, check out the Web Notes on the Strand7 site

http://www.strand7.com/webnotes/

- there are several downloadable articles with example models on damping, seismic analysis, etc.

http://julianh72.blogspot.com

 

[eqgeotech]

sorry I am not a student but I am using this software for the 1st time so I asked for ur assistance

 

[jhardy1]

For some examples of how to apply seismic spectral response in Strand7 - see Verification Problems VSR1 to VSR7 in the Verification Manual. (pdf copy should be in C:\Program Files (x86)\Strand7 R24\Verification on the hard drive where Strand7 is installed.)

See also Strand7 Web Note ST7-1.40.35.22 "AS 1170.4-2007 Earthquake Analysis in Strand7" which you can download form the website if you have an active maintenance account with Strand7:

http://www.strand7.com/webnotes/request/?w=ST7-1.40.35.22&origin=direct

Hope this helps!

http://julianh72.blogspot.com

 

[eqgeotech]

yes I got it, thank u for ur kind help and suggestions, expect u both to help further also.

 

[eqgeotech]

Do we need to provide node restraints at every node in the structure?

 

[IDS]

Do we need to provide node restraints at every node in the structure?

If you have plate elements with plane strain properties, these need to be restrained in the X and Y directions along the base and X only up the sides. No other nodes should be restrained.

If you are doing a 2D analysis you also need to set up a global freedom case, which should be 2D Beam (since you are using beam elements). This allows translation in the X and Y directions, with rotation about the Z axis, with the other three freedoms fixed.

Doug Jenkins
Interactive Design Services

http://newtonexcelbach.wordpress.com/

 

[eqgeotech]

IDS: I have some doubt in that, as I am using "transmitting base" condition so I am providing damping at the "bottom nodes" but I am bit confused for providing restraint conditions for the side and top nodes of the plate elements.

 

[eqgeotech]

I am uploading the image file of the model

 

[IDS]

Without knowing the details of how you are applying the loads I can't really give any specific advice, but general things you should consider are:

Restraints (in this case) are representing the body of soil outside the model. It follows that top nodes should not be restrained (other than the top corner at the sides of the model).

Side nodes are normally restrained in the horizontal direction only, but they should be far enough away from the structure that they don't have a significant effect. Three times the depth of foundation either side of the structure is a reasonable rule of thumb, so your model should be a good bit wider.

Also some aspects of the model look strange, but its hard to tell from a jpg, especially when you have the grid points displayed. If you want to upload an st7 file I'll have a (quick) look at it.



Doug Jenkins
Interactive Design Services

http://newtonexcelbach.wordpress.com/