how to use Table edition

[Anonymous]

Hi,

I'm trying to make changes to the model using the 'Table edition' tab and they don't seem to be observed correctly.  My model has prestress loads and I'm trying to change their value.  Steps are as follows.

1) begin with a solved model

2) in the 'Loads' table on the 'Table edition' tab, change the value for the prestress loads from e.g., 'N=1.00' to 'N=20.00' (fourth column - no heading)

3) Robot asks me if I want to make this change (yes) 

4) click on Analysis -> Calculations

The results I find are that the displacements are unchanged (I expect them to be different with this different prestress).  I also find that the member forces are different but not as expected.  Am I missing a "clear results" sort of function?  

I also find that if I delete these loads in the 'Table edition' tab, Robot does not converge without them (as expected - this is acceptable).  However then applying them with the modified values I want is again not correctly observed (i.e., same results as above).  Please advise.  

Thanks,

Keith

[Rafacascudo]

I have been studying this case  andwith a few modifications

Let me guess .

For a 20kip prestress ,vertical deformation at midspan will be 12.16 in and normal force will be -24.68kip ???

and yes,  for the original case (prestress =1kip) , deformation is 20.68 in and normal force is 14.52kip.

Is that correct???

[Anonymous]

Ahhh that's great!  And I didn't get to tell you that you do have a good sense of humor!  You'll probably be pleased to know that I too have been doing research - in my case it was searching for an existing post on this topic per your recommendation (I didn't find one so here we are). 

Yes, that's the correct solution.  It's a rather easy problem to solve by hand and one of my favorite "go to" problems when trying a new software (yes, I actually have favorite problems :).  I rather like it for the hanc-calc aspect and you might be surprised how many programs have trouble with this (I'm not impressed with 80 nodes but that's a different discussion).  I'd be pleased to share with you the exact solution if you like (i.e., the general equation) but it seems you may already have it or probably just solved it yourself.  Just let me know.  

How do you get this?  Am I using the 'Table edition' incorrectly? 

Also are there "tweaks/adjustments" made to your previous solution to get these (better) values?

Thanks,

Keith

[Rafacascudo]

It's simple. I will answer on your original post soon.

Right now I am busy . Doing some Yoga
😂😂😂😂😂
Send by cellphone

[Anonymous]

Hi all,

I received an email from <community@noreply.autodesk.com> with the question "Did you get the answer you needed?".  I don't see that question posted here but the answer is no, I haven't. 

I'm not clear if the problem I'm having with 'Table edition' not working is because prestress loads don't work correctly in Robot (in which case I wonder if I should start a new post on that topic - please advise) or if it's a problem with the way I'm changing the values.  One possible answer to this could be "you're changing the values correctly but prestress loads just don't work in Robot so the results aren't meaningful".  Yet another answer could be "you just need to click on xxx before/after making the change so that your new value is observed correctly".  I believe something in a form similar to one of these would answer my question.  

As an aside, I understand there were changes made to the forum this last weekend and one of them appears to be the exclusion of numbering assigned to the posts (e.g., Post 2, Post 3, ...)  I suggest this is not an improvement as the numbering was a convenient way to refer to specific posts within a topic. 

Thanks,

Keith

[Anonymous]

Hi all.  I'm wondering if @Rafacascudo or @Artur.Kosakowski or anyone else has been able to resolve this yet?  I suppose it must be a difficult one!  Any help is appreciated as we're currently considering Robot as a possible replacement for a product we currently use.  I'm basically just trying to find out if Robot works - not too much luck so far but I hope there are some smart folks out there with a simple solution to share!    

Thanks,

Keith

[Rafacascudo]

@Anonymous ,

I am sorry , but as I said before , only official support can clarify better about the issue with editing prestress loads using the load table.

In my tests ,it works , and ignores if you enter a negative value.It assumes a positive one

I would not rely totally on prestress load as it has some issues pointed on that thread by @alfredmx about force spikes.

Again I think official support has the word right now . @Artur.Kosakowski , @Rafal.Gaweda or @Pawel.Pulak  will surely help you on this issue

[Anonymous]

Hi @Rafacascudo, Thanks for your reply.  I appreciate your help and I look forward to hearing from the "official folks".  It's odd that it works for you though, are the results you get when changing to 'N=20' as you expect them to be?  I still get a displacement of 21.1734.  If you're getting better results, that suggests even more that it's something I'm doing wrong. 

It's been a little while now so I had to try again now just to be sure.  When I open your file, I see that the 'Deslocamentos' tab is already open and shows values.  This data does not change even after I execute steps 1 through 3 (i.e., especially step 3, which I would have thought would "clear" the results).  Should this tab still show data after I execute step 3 above?  Also the 'View' tab still shows the deformed shape too, is this normal?  Maybe that's part of the problem? It seems as if I'm missing a "clear results" type of function/button/setting.  

Also thanks for the link.  It helps me understand Robot better.  At first read, this seems very similar to a problem in the program by IES that I mentioned previously with "regular" forces - i.e., member loads applied at the ends of a member, not termed prestress but still handled incorrectly.  It's not uncommon.  Their "solution" is to use more sample points (ha! funny, right?).  If you create a cantilever in Robot and apply a concentrated moment (as a member load) at the free end you'll see that Robot too has this problem (i.e., zero moment at the free end where the load is applied).  If you show in the table results say N points, you'll see that N-1 of them show the correct moment but the end where the load is applied never shows the actual load.  Again for clarity, and especially for the "official folks", my problem is that the displacement doesn't change in Rafacascudo's model, not this rather tangential cantilever example.  

Thanks,

Keith

[Anonymous]

Hi @Artur.Kosakowski, have you been able to reproduce the problem at your end?  Am I doing something wrong?  Please advise.  

Thanks,

Keith

[Anonymous]

Hi @Rafal.Gaweda.  I'm wondering if support is able to provide help/direction/response.  Is this a bug in Robot?  If you're unable to help, please advise as to where I might find a solution. 

In case you haven't been following this thread, please find the attached model and try the four steps outlined in the first post to reproduce the problem.   

Thanks,

Ketih

[Anonymous]

Hi @Pawel.Pulak.  Rafacascudo indicated that you might be able to help me with this.  Is this a bug in Robot?  Or am I doing something wrong?  I appreciate your help.  

Thanks,

Keith

[Artur.Kosakowski]

Hi @Anonymous

I think you should allow for horizontal displacement of one of the supports to see the effect of axial force on deformation.

If I managed to answer your question(s) press the Accept as Solution button please. This will help other users to find solution(s) much faster. Thank you.

[Anonymous]

Hi, @Artur.Kosakowski, Thanks for your reply.  I really appreciate your help as I'm sure you know that support is an essential part of any analysis/design software. 

Unfortunately, I don't think I understand your suggestion.  Do you mean to allow a horizontal release in the direction of the members (i.e., global X)?  Won't this allow one support to approach the other?  That's a very nice nonlinear problem (whereby the solution has both supports drawn together to the same point and the two members are vertical) but that's not the problem I'm trying to solve.  The problem I'm trying to solve has both supports fixed (i.e., for translation).  There should be zero displacement at both ends and only the mid-span node is free to move.  

Also, why would it (sort of / almost) work for the given prestress "as-is" (i.e., without the release you suggest).  Please advise.  

Thanks,

Keith

[Artur.Kosakowski]

HI @Anonymous

IMHO for such situation to see the influence on the deflection the the cable should not be a 'straight' line with e.g. e2 value not being zero. You may want to switch off the large displacements so that the analysis converges to make a quick test.

If one or more of these posts answered your question, please click Accept as Solution on the posts that helped you so others in the community can find them easily.

[Anonymous]

Thanks for you suggestions.  I appreciate you kind help.  Regarding the non-zero e2, how can that be?  The model "works" as-is.  It currently gives a deflection in the solution (not the exact answer but somewhat close).  I'm just trying to change the prestress (Step 2 in my first post).  Are you saying that e2 can be zero with the first prestress I have (N=1.00) but e2 needs to be non-zero with some other prestress? (e.g., N=20.00)  What range would you suggest (e.g., e2 can be zero for N<5 but should be at least x" for a < N < b)?  Please provide a reference for this if you have one.  

Further to your suggestion of a non-zero e2 though, that's also not the problem I'm trying to solve.  The prestress in this problem is not eccentric.  Is this not possible?  

Regarding your suggestion to switch off large displacements, may I please kindly point out that this problem is unstable in a small-displacement world.  There is zero first-order stiffness in the transverse directions.  It must be considered as a large-displacement problem.  I don't expect to get a solution w/o considering large displacements.  

It's ok if you need to change some parameters of the model (e.g., number of elements, convergence settings, ...) but I don't want to change the "intent" (i.e., what it physically represents).  Unfortunately the two suggestions you've given of 1) release one of the supports and 2) use a non-zero e2 really give a different problem altogether - they represent something physically different.  I'm sure Robot can solve an infinite number of similar but different problems; I'd like to solve this one if possible. 

It seems like my error is somewhere in Step 2 of 'Message 1' above.  I listed the steps to reproduce the problem in that message because I know I appreciate that when investigating problems (hope you found it helpful).  Do you get a (meaningful) solution following those steps?  

Thanks,

Keith

[Pawel.Pulak · Accepted solution]

---

@Anonymous wrote:

Hi @Pawel.Pulak.  Rafacascudo indicated that you might be able to help me with this.  Is this a bug in Robot?  Or am I doing something wrong?  I appreciate your help.  

Thanks,

Keith

---

Hi @Anonymous,

Apologies for some delay of my response.

The effect you observe is not resulting from the bug in Robot but from the way the bar prestress load is implemented in Robot and from the properties of your test model.

The bar prestress load is defined in Robot by tendon tension force and the shape of the tendon – in general case 3 points of the parabola.

In the general case this load is internally replaced by the following set of equivalent bar loads (in bar local coordinates):

PZ uniformly distributed load resulting from parabolic shape of the tendon

FX concentrated forces at the ends of the bar corresponding to the tension of the tendon

FZ concentrated loads at the ends of the bar to balance the PZ UDL load

CY concentrated moments at the ends of bar corresponding to the eccentricity of tendon at these locations

In your model the prestress load is defined with the tendon along straight line without any eccentricities – so from above loads only FX concentrated forces are generated.

Moreover your model is a horizontal beam with fixed supports on both ends and with hinges (releases) on both ends and in the middle.

With such definition (fixed supports, none of them able to slide along the beam – already mentioned by @Artur.Kosakowski) the prestress load has no effect at all - appropriate loads are “self-balancing” or “lost”- applied directly to supports. Not only changing the prestress load from 1 kip to 20 kip does not change results – also complete delete of prestress load does not change them (of course providing nonlinear analysis is convergent). See this video.

Your model is somehow specific – it is originally unstable (2 hinges/releases on both ends and in the middle of collinear beam) and the stability is provided by considering large displacements effects resulting from deflected shape.

I guess you try to limit the deflection by adding the prestressing cable. But it cannot be done for such model using bar prestress  load in Robot. It is necessary to use negative bar elongation or negative temperature load. See this video.

Attached the modification of your model corresponding to such action.

---------------------------------------------
If this post answers your question please click the "ACCEPT AS SOLUTION" button (the button visible when logged to the forum). It will help everyone to find answer more quickly!

Regards,

[Anonymous]

Hi @Pawel.Pulak.  Thanks for your thoughtful and excellent reply.  This is a clear answer that I can understand and accurately addresses the problem.  I really appreciate the efforts of others and I'd like to thank them all again for trying but they just didn't seem to understand the problem like you do.   I really appreciate you taking the time to understand what's going on and offering meaningful help/support.  

Thanks,

Keith