Mesh problem on SDW 16 assembly

Simulation Resistance of materials
,
1

Hi all

I have an assembly on SDW that I can't mesh at all (some parts can't be meshed).

I tried changing the definition of the mesh but it has no effect.

If you have any ideas, I will be very grateful!

Thank you for your help.

Have a nice day


charpente_assemblage.sldasm
2

Good evening Chris59

We cannot do anything with the ASM file without the parts that go with it and especially without attaching the simulation study.

From the ASM, you have to do ==> file ==> pac and go (or take-away composition) ==> and indicate to attach all the files, as well as the results of the simulation study ==> ask that the output be done in ZIP.

Kind regards

PS: from the little I have for a few seconds when loading, I already have a little idea where the PB  comes from ;-)

1 Like
3

Hello

First of all, a big thank you for taking your time to deal with my problem!

Then, attached, the ZIP folder containing all the elements (the file to be processed is "assembly framework").

The objective of this simulation is to determine whether the cantilevered part of the framework will be able to support a load of 200 kg (evenly distributed on the latter). At the same time, I would like to determine the maximum load that this part can support (to give me an idea of the safety factor).

I am available if you need more information and a big thank you again!

Have a nice day

Kind regards 

PS: this is my first concrete use of SDW :-)


charpente_assemblage.zip
4

Good evening

I am watching and keeping you informed.

5

Good evening

Already for the mesh you have chosen a resolution in meters instead of mm.

  1. You have to simplify your ASM by removing all the screws because the mesh becomes too thin to be able to take them into account, especially since there is a hell of a bunch of screws). Screws and nuts are useless since you define the "global contacts" between the parts. Global should be understood as if you had a single body between two decks for example.
  2. Your part reinforcement1 has no material which makes the mesh you will have a failure in the calculation. You have plenty of other parts (poles) whose material is not defined.
  3. You indicated a force instead of indicating a distributed load, you did not select the "gravity"
  4. declare your posts as having all a fixed face (the wall). This will not be the case in real life. Say how your posts will be attached.
  5. Your load of 200 kg does not meet the standards for what needs to be staffed. The load is more like 500 kg per m²

Return the ASM by checking that all parts without exception have a declared material in the model.

For the rest we will see later ;-)

Kind regards

1 Like
6

Hello Zozo_mp,

Then:

- I updated my model for the fastening part. Note that the posts are fixed to the ground via plates and that the "MAT" part is fixed to another structure.

- I declared the material of the parts (AISI 304 for the whole).

- I updated the imposed trips and external loads.

- Finally, I created a new mesh by excluding all screws and nuts from the study. The network was therefore created. Now, I have a new problem running the study because the solver fails. 

Have a nice day

Kind regards

 


charpente_assemblage_maj.zip
7

Hello

Normally you must have another problem on the turntables  (turntable 1 and 2) because you have created a 3D thread which is never done for this type of assembly.

In addition, your turntable is 10 mm thick for M24 so it doesn't fit at all. In addition, if you do simulation on this assembly because then it requires a very fine mesh to take into account the nets, which is totally useless for several reasons.

 

There are other PBs  from my point of view in your design but hey, after all, you're not asking us for an opinion on them but only that your simulation succeeds.

I'm looking at your new file and I'll get back to you ;-)

Kind regards

1 Like
8

Hello@Chris69

The simulation was successful but on the condition that a finer mesh was put because the Traverse-7 part was in a mesh failure. You have to put a mesh size of 5.27 for the largest mesh and 0.26 for the smallest.

I don't know why a failure on only this part since this part is used in other places. But with the finest mesh, it's fine.

That's it, I've answered your question BUT there would be things to say about the simulation and also about the design

  1. You have a safety coeff of 2 which is not much for a gateway.
  2. Your bracing needs to be reviewed (in terms of content and form)
  3. The parameters of the simulation do not take into account the fact that if the columns are leaning against a structure (wall type) it is necessary to add a virtual wall with contacts without penetration, so as soon as the columns like ) buckle backwards it comes to rest on the other structure which limits or eliminates an aggravation of the buckling. Also putting it to have put the fixed beam does not represent reality.
  4. if the bridge receives personnel or potentially displaced loads, the CG of the load must be changed, i.e. it must be placed higher. The load is one thing but the CG of the load is something else that can interfere strongly on the result.

Hoping to have at least answered your initial request.

Kind regards

PS:  be careful the distortion on the image is deliberately exaggerated because in fact the displacements are only 7 mm. The image illustrates above all the potential buckling.

 


2019-12-16_14_04_37-solidworks_premium_2019_sp1.0_-_charpente_assemblage_maj.sldasm.jpg
9

Good evening Zozo_mp

The design and manufacture of this structure was carried out by a third-party company. Today, it does not suit us for various reasons, which forces us to modify it.

I have two questions:

1/ How do you determine the optimal limits of the mesh?

2/ How did you set the safety factor?

As far as bracing is concerned, I share your point of view! I will try to propose a modification of the latter in order to improve the safety coeff (our acceptance threshold being at 5).

In any case, I thank you very much for your time and your help!!

Kind regards

 

10

Good evening

I determine the optimum of the mesh in two ways, so the second in a somewhat empirical way.

  1. I look at the minimum thickness in your case which is 10 mm for the "platinum1" parts
  2. I look if two thin pieces are in contact because it is in these areas that the mesh is the most difficult to make, I put the meshes at 3/4 of the smallest dimension to favor the transition in the corners (without being obliged to give specifications for the strongly constrained areas).
  3. I look if there are small diameter holes (or things that have nothing to do in the simulation like screws, thread representations, etc...)
  4. So I choose a max value that corresponds to what you would need, for example, for your 80 mm tubes.
  5.  It must be borne in mind that who says that very fine mesh and the more there are a high number of degrees of freedom (several million arrive very quickly) because this generates very very long computation times.
  6. After that, the empirical method consists of launching the mesh and looking if there are any areas that either cause the system to crash or are too thin. and I chnage the settings of the Max mesh and the Min

To define the safety coeff there is a function provided for this, just ask for it ==> right click on the results function ==> choose define a route of the safety coeff ==> validate and the new section appears (see attached photo)

While waiting for your return, I made a simulation by shifting the load higher so as to have the notion of a CG that will necessarily be higher than the floor of the platform. The cg is at 1200 mm I also pushed a little granny in the nettles by putting a load of 4000 N. The result is a safety coefficient of 4 but with a small change in your settings.

If you want to go all the way and have something correct, he has to define the fixing points of the main horizontal beam "MAT" and also define what the posts are based on (a solid wall, a steel structure, etc...   Once these little things are set up, you will know if you are on target or not.

Kind regards  

PS: tell us if you want to go further in improving your simulation.

PS: attached is the image of the remote loading.


2019-12-16_21_16_08-solidworks_premium_2019_sp1.0_-_charpente_assemblage_maj__zzv2.sldasm.jpg