Basic FEA question 1

[transmissiontowers]

Sorry for the dumb question but I mostly do frame and truss analysis and only do FEA very occasionally. I use GTStrudl and their baseplate wizard to model and mesh up a flat plate with an angle welded to it held down on anchor bolts.

By hand I usually find the bolt loads and pick a bend line and sum moments about it to design how thick to make the plate by finding the stress at the top or bottom of the plate.

When I run the FEA and mesh up the plate and apply a load to the angle, I get results and I can see very large stresses at the tips of the angle and the stiffeners welded to it. The stress drops off quickly.

So my question is, do I make the plate so thick that there are no stresses above yield at any point in the mesh (even at the stress concentrations)? This is very conservative, but logic tells me that the plate will not fail just because a few nodes are twice the allowable yield stress.

I can assume a bend line through the point with the high stress and if I calculate the resultant forces on this cut, I can make the bend plane long enough (I usually assume 12 times the thickness as a limit) so that the P/A + M/S is below yield.

I'm thinking for the plate to fail in the real world, it will have to get plastic across the thickness so the plate tears.

My loads are due to hurricane wind so they are short in duration.

How do you FEA experts size the base plate thickness?

_____________________________________
I have been called "A storehouse of worthless information" many times.

 

[corus]

You will get high stresses at the tips because of the stress concentration effect of the detail there. Design codes nominally consider only primary direct and bending stresses, which these stresses don't fall under. The high stresses at the tips would be considered for fatigue assessment, and even then it's the nominal stresses away from the stress concentration/weld that you consider. You could assess them by plotting the stresses up to the detail and extrapolating the stresses so as to exclude the stress concentration effect of the juncture. That stress you'd assess against an SN curve for the parent material.

Tara

 

[rb1957]

would hurricane winds be a fatigue problem ? i'd've thought (possibly wrongly) that a code-strength hurricane is a pretty infrequent event.

i'd look at the plastic bending allowable of the plate.

the FEA is showing you peak stresses that don't affect a significant portion of the thickness. These stresses don't arise in reality 'cause the material is elastic ... it'll yield first. maybe do a non-linear FEA to convince yourself.

even if it yields thru thickness there could be plenty of reserve in the strcuture, as the structure plastically deforms and the load seeks out stiffer loadpaths.

 

[HankTexas]

I use FEA analysis quite a bit to size structures but only when standard code analysis or established engineering practice for a particular structure or connection is not available. That’s because code analysis is almost always based on actual tests that have been done to support the analysis procedure.

Allowable stresses or factors of safety for code requirements are based on loads that cause failure and not loads that yield the material even though the allowables are usually given relative to yield because that is an absolute reference. For instance it is well established that bolt bearing loads will yield the plate material in connections since the bolt diameter is less than the hole diameter which creates a point load until the bearing area on the plate deforms enough to carry the load. However the failure load will be close to the total bearing area of the bolt times the ultimate bearing strength of the connecting plate.

So to answer your question I always use the P/A + M/S formula for sizing base plates instead of the FE analysis if the base plate is a simple design. I’m assuming when you say limiting the stresses to below yield that you have applied appropriate load factors to the loads before calculating the stresses. I have seen several different methods for determining the assumed width but the one I have seen used most often is twice the distance from the centerline of the bolt to the edge of the stiffener plate or structure plus the width across the flats of the nut. This assumes a stress distribution length based on a 45 degree angle from the nut to the structure. I did my masters thesis on this subject and found that to be a reasonable assumption based on hundreds of base plate FE analysis. If you look at the stresses from the FE model you should see a section of higher stresses at the base of the structure that is about that length. I also found that if you can place the bolt as closely as possible to the stiffeners or structure base the anchor bolt diameter and the base plate thickness will usually be close to the same.

Hurricane winds are not considered fatigue loading since they are usually base on a 50 year storm and most structures are designed for a life of 50 years. Therefore very few loadings would be applied to the structure at that extreme wind case.

 

[transmissiontowers]

Thanks for the explanation. Yes hurricanes are a 50 year event and the max wind is not sustained for very long and there is not much if any fatigue. Our loads do have overloads on them, so we design the plate in bending to be below yield and do not use plastic design. On a "normal" plate with 4 bolts and an angle sticking out, I just calculate the bolt loads and assume a bend line and sum moments about that plane and size the plate for M/S.

My particular plate uses a 10x10x1.25 angle (actually 2 plates welded together) plus 3 stiffeners welded to a plate with 16 bolts in a round pattern. A picture is attached for those that want to see. This particular plate will be 8 feet above salt water so we are going to use 316 stainless bolts 2.25" in diameter. It is a base shoe on a 340' tall transmission tower.

I meshed it up in FE to get an idea of how thick to make the plate and I came up with high stresses at the corners of the stiffeners. I then used the FE program to output the P and M on a cut and I did P/A + M/S to determine that the average stress on the bend-line was under yield.

My other dilemma is how long to make the cut. If I make the cut the width of the plate the stress is very low. If the cut is only 4 inches centered on the high stress point, the stress is above yield due to the high stress concentration.

I'll post a stress contour to illustrate.

I couldn't figure out how to attach more than one file so I'll do another post to get the plate detail.

_____________________________________
I have been called "A storehouse of worthless information" many times.

 

[transmissiontowers]

Here is the plate detail.

The purpose of my question was to get an idea on how to handle complicated base plates with multiple bolts and many possible bend lines.

_____________________________________
I have been called "A storehouse of worthless information" many times.

 

[crisb]

If I was modelling this using FEA, I would probably carry out a contact analysis including the concrete base, as well as the base plate and angle, and all the bolts (inclusing any pretension). This will probably introduce another plastic hinge close to the line of the bolts and substantially reduce the moments at the angle tips. From your stress plot I doubt you have included this effect. I would then run the analysis at working loads and look at maximum stresses......then run it at ultimate including all safety factors, when I would be quite happy for all the plastic hinges to form.
Having said all of that I would do this type of analysis using hand calculations most of the time, except for a very rare check on an unusual case by FEA.

 

[transmissiontowers]

I guess I forgot to mention that the plate sits on leveling nuts on the anchor bolts and there is a 2 to 3 inch gap between the bottom of the plate and the top of concrete. Our construction people cannot pour concrete to close enough tolerance to have the same elevation so we use leveling nuts to set the elevation. The footings are 100' apart. The bolts are not pretensioned but the nut on top and bottom of the plate clamp it tight so the 244 kips of shear is transferred through friction to the bolts and the 831 kips of compression tries to push the angle down through the plate.

And yes, I usually do these base plates by hand and have written some FORTRAN programs to size the plates on the tubular poles I usually have on the plates.

I just wanted to try out some FEA on a little more complicated angle with stiffeners.

_____________________________________
I have been called "A storehouse of worthless information" many times.

 

[corus]

The maximum stresses from your model are probably an underestimate due to the relatively coarse mesh, but then again it appears you've used shell elements so the shell edge alone will give rise to 'infinite' stresses. Plotting the stresses up to that 'infinite' stress will allow you to make a judgement as to the amount of peak stress and the amount of local primary plus bending stresses at the toe. Generally local stresses are limited to yield in the codes I've used, whereas general primary plus bending are limited to 0.6 Yield.



Tara

 

[rb1957]

well, you're not sure about his mesh, are you ? i didn't see it posted.

what we have learnt is, i think, that the high stress at the base of the stiffeners is the only load path for load into the base plate which makes the stress peak somewaht more serious.

if the peak stress is only a small %age of the thickness probably still no big deal.

i'd encourage you to do a material non-linear analysis, and to refine the mesh probably way more than you ususally might.

right now you have the plates sitting on top of the plate (and welded). would it help to cut slots in the base plate so that the plates could pass thru and get welded on both faces (of the plate) ?

 

[HankTexas]

I agree with rb1957, you don't have a very good load path into the angles. It appears to me you are going to get high stresses at the base of the angles. If you refine the mesh, as rb1957 suggested, you will find out if the stresses converge to a maximum or if they are mathematical singularities. You need to know this.

I don't know your restrictions but could you use say a 6" section of round pipe or rolled plate that had a diameter slightly less than the anchor bolt circle as a stiffener, then run stiffeners from the angles out to the pipe? This would give you a much better load path if you can do that.

 

[corus]

Here's the mesh overlayed on the results rb1957. It was posted earlier.

Tara

 

[rb1957]

apologies ... i only opened the drawing attmt

it is a coarse mesh. two questions arise ... the base of the plates look like they're completely in tension (pink), and 2nd, why the comment "stiffener attached here" pointing at one point; ok, he probably means all the stress peaks, but aren't the plates welded all round ? 3rd question, 2D elements or 3D ?

 

[rb1957]

4th, not sure i like the triangle elements at the tie-down fasteners. distort the mesh if you want, but i'd use a couple of elements to avoid highly skewed quads.

 

[transmissiontowers]

Sorry for the confusion. The eMail notification is not working for me on this thread.

The base plate is 48" square and each plate element is 1 inch square or thereabouts. I use GTStrudl and their new Base-Plate Wizard that automatically meshes the plate around the angle and stiffener attachments. My Snagit (great program BTW) screen shot note was pointing to the high stress point, and yes, the angle and stiffeners are full penetration welded to the top of the plate. The FE elements are SBHQ6 which is a 2D plate bending element with 6 DOF at each of 4 nodes(according to the manual).

The plate in my AutoCAD detail is round but it was easier to make it square in the FEA run so that may add to the confusion.

The plate model was 5 or 6 inches thick so I'm not sure if the plate elements are the right choice since the plate is so thick compared to the mesh size of 1 inch. If I were doing a real rigorous FE analysis, I would think a 3D solid element would be more appropriate with 6 rows through the plate thickness, but I was just trying to get an idea of how thick to make this base plate to verify my hand calculations.

The original plate used 75 ksi rebar bolts (8 on a smaller bolt circle) and had a capacity of 1950 kips. Since the new plate was to use stainless steel bolts with 40 ksi yield, I had to use 16 bolts on a larger bolt circle which produced bigger bending moments and the 6 inch plate. We have since discovered that we could get by with only 831 kips of compression, so the plate can get thinner.

I had thought of cutting a slot in the plate but the 10x10x1.25 angle intersects the plate on a double bevel (aren't transmission towers fun?) and a slot in a 6 inch thick plate would be too tough to do at a double bevel.

I didn't design the original plate but I believe the stiffeners are there to give more weld area because there is relatively little moment in the connection and the original 8 bolts were much closer to the angle. I used more bolts and spaced them farther out. I probably should have used a double row of bolts to get them closer to the load. The original 8 bolt plate was 3.5 inches thick with a 20" bolt circle IIRC.

It may have been a wasted effort, since the foundation engineer can't get an economical pile group to work for our lousy soils at 831 kips. Forty feet of muck below 10 feet of salt water must be hard to deal with.

For those that saw this on the news in Texas, this is the electrical crossing tower over the Houston ship channel that was hit by the barge and closed the channel for 3 or 4 days. The barge owner is going to pay for the restoration but we were going to reroute the line a little and use a different replacement tower.

Sorry for the long dissertation, but I was trying to answer everyone's questions and suggestions.

_____________________________________
I have been called "A storehouse of worthless information" many times.

 

[rb1957]

48" sq and 5" thick ... i'd definitely use 3D elements. i guess with full penetration welds you'd have nodes common to the base plate and the stiffener plates all through the thickness (rather than just at the edges).

from your screen shot, it looks as though the angled plate doesn't intersect the corner ... the diagonal elements look to stop short of the corner created by the other two plates. using 2D elements is making the stiffeners appear narrow on the base plate ... instead of being 1" wide they're joining the baseplate on a line ... i think this is making the stress peak in the base plate more intense.

 

[transmissiontowers]

Yes, I'm just getting a handle on this plate analysis and trying something new (to me anyway). I've been designing base plates by hand since the mid 1970's but with the new Base Plate Wizard in GTSTRUDL, it is pretty easy to generate a FE model but I get perplexed when I view the stress. I see if I ignore the big stresses at the points where the stiffeners and toes of the angle attach to the plate, the plate thickness is OK.

I'm used to finding the bolt loads and solving for the thickness that makes the plate bending stress less than yield.

_____________________________________
I have been called "A storehouse of worthless information" many times.

 

[crisb]

Just wondering if the very high stresses at the tips of the angles could be caused by the way GTStrudl implements the base plate wizard?

For example if the incoming member extension is very short, rigid, or non existent, this will cause an unrealistic stress regime at the intersection. Also its possible that the program applies the forces and moments as a rigid link between an arbitrary point and the end of the member, rather than applying the correct axial and bending stresses at the end of the member. I do not know but would probably be wary of using the base plate wizard without an independant check on how it works.

 

[transmissiontowers]

I'm going to the annual User's Group Meeting in June and will ask the developers then. There are several choices on how the angle is attached to the main plate including having it made out of plate elements. I chose the method where the angle was a rigid solid since I was interested in the base plate and not the angle.

The wizard is just a preprocessor that generates the FE model and boundary conditions so you can run the model in GTSTRUDL.

_____________________________________
I have been called "A storehouse of worthless information" many times.

 

[crisb]

If you have a moment it might be interesting to try rerunning the model with the angles and stiffeners having correct elastic properties (not rigid), and the length of the extension comparable to the largest dimension of the base plate.