Algor V17 - Modelling a press frame 1

[mcfridge]

Hello, I was just wondering if someone could help me set up the model for this? I have a frame with a distributed load across it. I'm just trying to simulate my case accurately, it doesn't have to be super technical or anything. I drew the frame in Solid Edge, saved it as a .stp file, and imported it. It meshed without any errors, and I've been able to run a few different simulations without problems. The frame is shown below.

http://us.a1.yahoofs.com/users/422874fbze403644a/f499/__sr_/4bcfscd.jpg?phYejHEB2q1rQv.7

As you can see, the I-beams in the middle (support) are facing the wrong way, and I want to see how much they are actually going to bend/flex in the middle and how it contributes to the overall deflection. I'm trying to figure out which surfaces I should fix or what I should do to set up my simulation (when I fixed the bottom surface of both of the bottom beams, it came out how it should look, but the bottom beams had no deflection). Also, the distributed load is only applied to the inside surface, but I had to apply it to the entire surface as shown below:

http://us.a1.yahoofs.com/users/422874fbze403644a/f499/__sr_/e819scd.jpg?phYejHEBlub3oStI

If this isn't clear I can try to explain it better. Thanks.

 

[GBor]

mcfridge,

I can't seem to access the websites. I'm guessing it is the spaces between / sr /. I think with the pictures, your explanation is probably sufficient. Without them, it's difficult.

Garland

Garland E. Borowski, PE
Borowski Engineering & Analytical Services, Inc.

http://www.borowskiengineering.com

 

[mcfridge]

Whoops, sorry. Maybe these will work.

http://ca.pg.photos.yahoo.com/ph/mcfetric/detail?.dir=f499&.dnm=4bcfscd.jpg&.src=ph

http://ca.pg.photos.yahoo.com/ph/mcfetric/detail?.dir=f499&.dnm=e819scd.jpg&.src=ph

 

[GBor]

Great, that helped. I'm not sure I understand your statement

As you can see, the I-beams in the middle (support) are facing the wrong way

and I have a couple of comments:

When you mesh these structures, you need to define a smaller mesh size. One element across a flange will not give accurate results. If you are automeshing, then you need to use the mid-plane option and you need to set up different parts in your CAD model where flanges overlap (this defines them as a different part when they are imported and gives you the opportunity to define a different thickness at that point. There will likely be some issues with mid-planing since the software will place the mesh at the midpoint of the CAD solid plates. This means that in the areas where the flange is "double-thick", the mid-plane mesh will be offset from regions where it is a single flange thickness.

I'm not sure what's going on with your pressures. Clearly, something isn't quite right. How did you apply it? Normally, I would swith my selection to point and surface so that a single mouse click selects the surface of interest. Then right click and add a surface load from the right-click menu. I can't really tell what surface this load is added to?

One final comment, this structure is pretty easy. I might consider modeling it in FEMPRO. Again, some "bean-counting" to make sure meshes line up, but it would be a great modeling exercise.

Garland E. Borowski, PE
Borowski Engineering & Analytical Services, Inc.

http://www.borowskiengineering.com

 

[mcfridge]

Hey GBor,

Thanks for the help! When I said that the support I-beams (the 2 beams at the ends holding the 4 beams apart) are facing the wrong way, I meant that they were turned in the weak direction. The top and bottom beams are flexing away from the centre, and I know that these two support beams are going to bend, and I was just wondering if there was a way to figure out how it would contribute to the overall deflection. I was also wondering if there was a way to isolate the single beam to determine how much it had bent and the stress on it.

As for the pressures, I did what you talked about and applied the load to the entire surface: I applied a downward pressure to both surfaces of the bottom beams, and an upward pressure to both surfaces of the top beams.

I'm just trying to get an idea of how much those support beams are going to bend. When I fixed the bottoms of both of the bottom beams, it came out (in an exaggerated way) how I thought it would look (with the middle of the support beams bending towards the middle while the top and bottom flex outwards), but the bottom beams had no deflection (which isn't exactly what I want, since the beams are in fact sitting on top of steel caster wheels). And the support beams were also a pink colour showing they had no deflection or stress?

 

[GBor]

I understand a little better, so let me see if we can get you headed in the right direction.

First of all, your boundary conditions: Instead of using a surface boundary condition, you can box select the nodes on the bottom surface of the bottom beams and only at the end where they are supported by the casters. Right click once you have the desired nodes selected and select "add-nodal boundary conditions". A dialog box will come up and I suggest that you only select the direction of the load (so, if your beams are lying in the x-y plane, fix the z-direction. This will allow the ends to move freely, but only in the x-y plane. If the casters are directional, you can also limit the direction perpendicular to their movement so that the ends of the beams can only move along the beam axis.

Secondly, the middle supports: There are a few ways to determine the stress and deflection in these beams alone, but it depends on your model. If you have the beams in their own parts, you can select the specific part in the menu on the left, right click, and hide it. Only the visible parts are considered when the stress dither is performed. If they are not in their own parts, you can still box select surfaces or lines and hide them with the right click menu...this doesn't work quite as well, because it is sometimes difficult to select all of the correct surfaces. If you can determine which surfaces are remaining that you don't want, you can select them under the part in the menu on the left, and hide them in the same manner that I suggested for the parts above.

You can also reset the various scales on the legend under "display Options". I often set the scale to something like 0 to 35000 for the max/min, but if the stress is low enough (which is what I think to be the case in your situation), I will drop it down as needed. If I am looking at Max Prin stress, I will, of course, set the lower end to negative.

I don't fully understand your model, but I think I'm starting to get it. Part of my lack of understanding is the graphic for the pressure vectors. I can't really see which surfaces you are trying to load.

Garland E. Borowski, PE
Borowski Engineering & Analytical Services, Inc.

http://www.borowskiengineering.com

 

[mcfridge]

Hey GBor!

Thanks a lot for your help, if I lived near you I would definately owe you a case of beer.

This isn't my setup, but it is very similar to what I have done:

http://www.skibuilders.com/howto/equip/press02.jpg

That might help you see better what surfaces are being loaded. The "bladder" (firehose) is inflated to create pressure, so it pushes down on the bottom surface, but also pushes back up against the top mold, so it is pushing on the top surface as well.

Also, the beams are all separate parts, so I will have to try what you suggested. I tried doing something similar where I selected (I think) "show results" on the individual part & one of the nodes on that part, but it still came up as zero.

 

[GBor]

I remember seeing something like this on one of the other forums (perhaps the FEA forum). Now I understand! At least, I think I understand...we don't do much snowboarding or snow skiing around here...and I really don't know how water skis are made. I was built for under the water (SCUBA).

Let me know if you keep having trouble. You can get an e-mail address from my website and e-mail me an archive if we need to get serious.

Garland E. Borowski, PE
Borowski Engineering & Analytical Services, Inc.

http://www.borowskiengineering.com

 

[GBor]

McFridge,

A thought just occured to me...this is perfect for a quarter-symmetry model. It would dramatically reduce the time effort you put into it. If you can imagine, all deflections should be symmetric meaning that the top and bottom should basically form bowls. Deflection on the left should equal deflection on the right. Because of this, you can use a set of symmetry boundary conditions. If you think this would help in any way, let me know and I can explain in greater detail.

Garland

 

[mcfridge]

I think that would help a lot GBor, what did you have in mind? You are right about the top and bottom forming bowls, and the support beams will form sideways bowls (if that makes sense).

This picture shows it in an exaggerated way of how it should look after the loads are applied:

http://ca.pg.photos.yahoo.com/ph/mcfetric/detail?.dir=f499&.dnm=a170scd.jpg&.src=ph

 

[GBor]

Do you see how you are getting an exaggerated "v" cross-section in the support beams. It is because you only have 2 elements down the web. If you are using node-limited demo software, you can quadruple your node count and still stay under the node limit by cutting your model into a quarter symmetry. Basically, cut them model in half between the longitudinal I-beams (the long ones running top and bottom) and cut it again across the midpoint of those longitudinal beams. Your model is now "quartered". If you delete three of those quarters, you are left with a quarter symmetry model. In SolidWorks (I'm assuming it is similar in SolidEdge, I have a feature that I call "analysis cut" which I can suppress in the CAD model configuration and unsuppress in the analysis export configuration.

Now, when you build the model, you place different constraints along those cut lines. Let's say that your long beams are oriented so that the axis of the beam lies along the z-axis and the web is parallel to the x-axis (I can't tell from the pictures because the origin icon doesn't show). That means that your first cut (down the center of the beams) would be in the x-z plane. If you can imagine, any deflection that would occur to the left of the x-z plane would pull to the left, but if you had the full model, any forces pulling to the left would be countered by forces pulling to the right. Because of this, that centerline can't come off the x-z plane. So, you boundary conditions along that line should limit y-translation. Similarly, it would limit x and z axis rotation. Using this same logic, the second cut would be in the x-y plane and would not allow any z-axis translation along this line. It would also limit the x and y rotations. Where these two planes of symmetry cross, the only motion that would be allowed would be vertical (in the x direction).

You will get the same results on a much smaller model. You just have to understand that the same deflections are occuring in the other parts of the structure. Look at your current model and you will begin to see what I'm talking about. Generally, the middle will have the greatest deflection and the color pattern will be pretty concentric circles radiating outward. This is an indication, although not proof, that your model is symmetric.

I would encourage you to look at whether or not brick elements is the right choice for your model (it looks like you are using bricks) and I would encourage you to increase your element count down the web and across your flanges. Right now, I think your results are going to be poor at best because your mesh is too coarse. Generally, when performing FEA, you should perform a mesh-sensitivity analysis. In short, run the model and get some answers. Document those results and either increase the mesh density by remeshing, or turn on mid-side nodes on your existing model. If the results change by more than about 10% (5% on a really uncomplicated model), you probably need to increase your mesh density to achieve a good convergence.

Garland E. Borowski, PE
Borowski Engineering & Analytical Services, Inc.

http://www.borowskiengineering.com