AnsweredAssumed Answered

Numerical Node/Displacement List Incomplete

Question asked by John Willett on Dec 15, 2012
Latest reply on Feb 22, 2013 by Anthony Botting

Like • Show 0 Likes0
Comment • 17

I'm considering a purchase of SolidWorks Simulation Premium. A friend demo-ed his copy on a static-deformation problem of interest to me, but we can't get it to do what I need. Whenever we ask for a list of nodes and displacements, we only get a partial list in the resulting CSV file. Althuogh the graphical results look complete and credible, a large fraction of the part's volume, and the vast majority of its nodes (judging by node numbers), are missing from the exported file.

Can SolidWorks realiably export numerical results? If so, what are we doing wrong? Thanks in advance -- John Willett

Anthony Botting Dec 15, 2012 2:56 PM

Correct Answer

Hi John: Perhaps it's an issue in a particular version of the software? I am running SW 2012, SP2. I did note that I had to select the "Advanced Options" panel and press on the button there labeled "range", in order to get every single node. I attached a screen shot of what I see. I was able to verify the *.csv file does show every nodal point when I opened it into Excel. Let me know if it still does not work.. Tony

See the reply in context

No one else had this question

Outcomes

17 Replies

Anthony Botting Dec 15, 2012 2:56 PM
Unmark Correct
Correct Answer
Hi John: Perhaps it's an issue in a particular version of the software? I am running SW 2012, SP2. I did note that I had to select the "Advanced Options" panel and press on the button there labeled "range", in order to get every single node. I attached a screen shot of what I see. I was able to verify the *.csv file does show every nodal point when I opened it into Excel. Let me know if it still does not work.. Tony
Like • Show 1 Like1
Actions
John Willett Dec 16, 2012 11:17 AM
Mark Correct
Correct Answer
Anthony -- Thanks very much! We now see that there are various pre-defined options for (apparently five-column only) output files. Two more questions, if I may:

1) Do you (or does anyone) happen to know if there is an option for user-defined columns in an output file?

2) Is there a general User's Guide or Technical Reference Manual that explains all the gory details? We're not finding answers to many of our quetions in the built-in help files?

Best Regards. -- John Willett
Like • Show 0 Likes0
Actions
- Anthony Botting @ John Willett on Dec 17, 2012 10:41 AM
  Mark Correct
  Correct Answer
  Hi John: For 1), I do not know about that. For 2) I am aware of a technical document called "COSMOS/M Theoretical Manual" (or a name simliar to that). It shows exactly how the equations are solved and how the shape functions are formulated for each element type. However, I believe you're after something more about the output formats and control for that. I am not aware of such a document. It is likely there is not one since, I recall years ago, the developers decided to go 'all-electronic' with the documentation.
  The best resource to obtain this information would be your VAR. They are obligated assist you by direct query to the developers via a "Support Request", opened in your name.. I hope that helps - it's likely the very best route you can take at this point.
  Sincerely,
  Anthony
  Like • Show 0 Likes0
  Actions
  - Laila H @ Anthony Botting on Feb 22, 2013 9:58 AM
    Mark Correct
    Correct Answer
    Excuse me Anthony, do u have any idea where we can get this manual "COSMOS/M Theoretical Manual"?
    Like • Show 0 Likes0
    Actions
    - Anthony Botting @ Laila H on Feb 22, 2013 12:15 PM
      Mark Correct
      Correct Answer
      I am only aware of your VAR as a resource. It used to be (10 years ago!) for sale as a hard-bound book, but now it may only be available as a PDF file. Please try your VAR as the only resource of which I'm aware to obtain that document. - they should be able to obtain it from the developers. Good luck. -Anthony
      Like • Show 0 Likes0
      Actions
- Bill McEachern @ John Willett on Dec 17, 2012 10:50 AM
  Mark Correct
  Correct Answer
  I am unaware of any options to specify output columns. However, you can go to all the results you want and export the items of interest into excel and use cut copy paste to put wahtever you want into a single excel spreadsheet. It might not be elegant but at least you can get what you want in all likelihood. Maybe you should let us know why you want it and what you are trying to do. There may be a better way to get where you want to go than the route you are specifiying. Maybe, maybe not......
  Like • Show 0 Likes0
  Actions
  - John Willett @ Bill McEachern on Dec 17, 2012 12:49 PM
    Mark Correct
    Correct Answer
    >>...you can go to all the results you want and export the items of interest into excel...<<
    
    Bill -- This is exactly where we are having problems. Other than the relatively few (and rather inscrutable) pre-defined output options that we have found on the "List Results" page (as kindly indicated by Anthony), we have not found a way to display/select specific numerical results (indexed by node number so that they can be aligned in Excel, as you suggest). Can you be a little more specific about how to "go to all the results you want?"
    Like • Show 0 Likes0
    Actions
    - Bill McEachern @ John Willett on Dec 17, 2012 1:27 PM
      Mark Correct
      Correct Answer
      what do you want other than stress, strain and displacement? Where are you going with this? Why do you want it?
      You can try looking in the .out file. I did notice that in reaction forces, it doesn't list all the nodes - just the ones with the actual computed quanities which might be a bit problemmatic, but not insurmountable.
      Like • Show 0 Likes0
      Actions
      - John Willett @ Bill McEachern on Dec 17, 2012 2:18 PM
        Mark Correct
        Correct Answer
        >>You can try looking in the .out file. I did notice that in reaction forces, it doesn't list all the nodes...<<
        
        Bill -- I just didn't understand your meaning in the previous quate. We'll take a look at the .out file and try to make sense of it...
        
        We're doing a relatively simple, static, stress/strain problem in 3D. Thanks to Anthony we now know how to get (Node, X, Y, Z, URES) and (Node, UX, UY, UZ, URES) for all nodes by selecting options in the somewhat counter-intuitive List Results window. We also stumbled on a way to get (Node, X, Y, Z, "Value") on one of the surfaces of interest, but we're not sure how to determine what "Value" is shown there. Given the three files described above, with some effort we can get what we want by manipulating them in Excel to match up (UX, UY, UZ) from the second file with the specific nodes on the surface from the third. It seems that the whole process should be more flexible and more transparent: but if no, so be it.
        
        Anyhow, thanks for taking the trouble to reply. It will be a fabulous program when we finally figure out how to use it... -- John Willett
        Like • Show 0 Likes0
        Actions
        Bill McEachern @ John Willett on Dec 17, 2012 2:29 PM
        Mark Correct
        Correct Answer
        Yeah, I just checked the .out file only has summary info now so it won't help much. The list selected command for any plot will get you a value (of whatever is being plotted), node numbers and coordinates (if selected). You can add as many surface as you want into that to get out specific values.
        I am still wondering why this is so important given that you can look at the graphical data. Why the focus on the tabulated data? List selected will also plot data - say along an edge or in the probe tool - tool for selecting a specific set of nodes fromthe graphics area.
        The reason it is the way it is as there has no been a lot of demand to get better tools to look at the tabulated data. Most people are happy to be moving away from it.
        Like • Show 0 Likes0
        Actions
        John Willett @ Bill McEachern on Dec 17, 2012 5:45 PM
        Mark Correct
        Correct Answer
        >>I am still wondering why this is so important given that you can look at the graphical data. Why the focus on the tabulated data?<<
        
        Bill -- Well, in our case we need the normal distortion of one surface of an object (the optical surface of a mirror) in numerical form in order to compute deviations from a best-fit sphere, parabola, or whatever is the ideal surface (to account for re-focusing the optics) in wavelength units. Having done that, we need the peak-to-valley and RMS magnitudes of the resitual across that surface. I hadn't occurred to me that more engineers don't have similar needs. Perhaps there's a way of using SolidWorks to do this subsidiary computation and spit out graphical results, but we haven't gotten that far; so I am headed for an external analysis in Excel, Mathematica, or some such...
        
        Anyhow, thanks for the additional suggestions! -- John Willett
        Like • Show 0 Likes0
        Actions
        Bill McEachern @ John Willett on Dec 18, 2012 3:14 PM
        Mark Correct
        Correct Answer
        Hi John,
        If you plot the displacement component you are interested in - displacement plot for x. If you select the "list selected" option under the plot menu (RMB (right mouse button) on the plot in the tree) and then select the surface of the lsurface you are after, hit update in the dialog. It will produce a list of nodes for all the nodes on that surface along with the x displacement. Do that for all the components and then put the spread sheets together and it should get you what you want in a logical fashion, albeit with a little more work than you might ideally want. You will get the componet value (ie x displacement), the node number and its underformed (mesh) coordinates. Should be pretty easy to get what you want then, no?
        Like • Show 1 Like1
        Actions
        John Willett @ Bill McEachern on Dec 18, 2012 3:18 PM
        Mark Correct
        Correct Answer
        OK, Guys, here are two more specific questions about the output options:
        
        1) What option determines whether you get (node, X, Y, Z, UY) or (node UZ, UY, UZ, URES)?
        
        2) In the latter case what do the advanced reference options (e.g., "Front Plane," "Top Plane") actually do? It appears there is some sort of coordinate rotation going on between them -- the order and sign of some of the U components changes. (What we want is to assure that the U components are in the same coordinate system as the node-location components.) This section of the built-in help is more confusing than helpful...
        
        Best Regards -- John Willett
        Like • Show 0 Likes0
        Actions
        Anthony Botting @ John Willett on Dec 18, 2012 5:08 PM
        Mark Correct
        Correct Answer
        Just a note:
        On 1) If you right click on the "Results" folder and choose "List Stress, Displacement, Strain", you can output <Node #, UX, UY, UZ, URES>, but not the starting coordinates of the nodes.
        If you right click on a plot (say "Displacement URES") and choose "List Selected", you can output <Node #, URES, X, Y, Z>.
        
        On 2). Yes, any other plane you select will do a coordinate transformation/rotation. The "Front" plane (at the assembly level, if you are using an assembly) is supposed to be the referenced "global" coordinate system for a collection of parts. Likewise the "Front' plane is supposed to be the referenced "global" coordinate system for a single part.
        Hope that helps.
        Like • Show 1 Like1
        Actions
        Anthony Botting @ John Willett on Dec 17, 2012 4:58 PM
        Mark Correct
        Correct Answer
        Hi John: just a note that I thought of, which you might be able to do. If you have the product called "SolidWorks Simulation Premium", there is the old interface known as "GeoSTAR", which should show up in your Windows Programs list. Anyway, you can port the SolidWorks Simulation model into "GeoSTAR", run it there, and the default information in that program's *.OUT file normally contains every single node's displacement component, and every single element's stress and strain component in a text format. Just a thought.
        
        You might need to speak to your VAR about using it, however. It has a "command-interpreter", where you can type-in commands and also pull-down menus to have it automatically type-in the commands with a mouse click. I originally learned COSMOS on that interface, but I have not used it in quite a while. It is still supported by the developers, but they are not currently "developing" it - meaning, no updates to it.
        Like • Show 0 Likes0
        Actions
        John Willett @ Anthony Botting on Dec 17, 2012 5:46 PM
        Mark Correct
        Correct Answer
        >>...there is the old interface known as "GeoSTAR"...<<
        
        Thanks again, Anthony. I'll pass that along to my colleague as well. -- John Willett
        Like • Show 0 Likes0
        Actions
        Anthony Botting @ John Willett on Dec 18, 2012 5:13 PM
        Mark Correct
        Correct Answer
        Hi John:
        I just ported a model from SW Simulation into GeoSTAR, ran it there, and it still works! Yes, every single component of stress, strain and displacement is there for every single node and element - including total strain energy and error estimate, in a nice list in the <problemname.OUT> file!
        However, the starting coordinates of the nodes are not there. The starting coordinates are in the saved output file from SolidWorks Simulation in a file with a "*.geo" extension.
        Perhaps, since everything's in those two files, it would be easiest to parse if you're coding parsing commands on a text file. Just a thought.
        Tony
        Like • Show 1 Like1
        Actions

Incoming Links

Re: Definitions of the "Standard Planes"?

Numerical Node/Displacement List Incomplete

Outcomes

Related Content

Recommended Content

Incoming Links