Learning Forum

[MickMack]

Hi Guys,

I am trying to replicate a study from the literature by Styles et al (2016) whereby i must create a simulation of a connection namely the vertical tie as shown below. I could use some assistance in assigning the SOLID to be used.

[1shan]

In addition to changing the element order to linear you also need to add a command snippet under the respective geometry object - 'et, matid, 185'. Also, these are 2 useful videos you might want to check - https://www.youtube.com/watch?v=UzFh_UbUF4k and https://www.youtube.com/watch?v=gRUeyWTwJ2g.
Regards Ishan.

[MickMack]

I have inserted this command under the geometry object and i keep getting the same error, as shown below regarding "switching to a different shape is not allowed". I have tried a number of different variations including adding KEYOPT2(3), and changing the mesh from linear to quadratic.


I also inserted the command separately into pre-processing but it made no difference.


Could you offer any further advice?

Many Thanks Michael

[1shan]

Solid 185 is a hexahedral element and the mesh probably contains some tetrahedral elements which is causing the error. Use mesh controls to create a pure hex mesh on the part to which the snippet is added.
Regards Ishan.

[MickMack]

I have been able to create the solid185 without the use of the command snippet. However i have tried to insert a command snippet under the geometry to change KEYOPT 2(2), which appears to be the default to KEYOPT 2(3).

Could you advise how to do this i have tried a variety of different commands but keep getting errors as shown below, stating 0 is not a valid id number.



Regards Michael

Details of creating 185 solid
To create the hexahedral mesh necessary as indicated in a previous post i had to slice the solids in the design modeller to create simpler solid with sweepable bodies. I followed the process shown in this video https://www.youtube.com/watch?v=oOAx4j3D2rc, shown in the first pic below. Once this was done i returned to mechanical and automatically generated my mesh ensuring that the element order selected was 'linear'. Once i sent the model to the solver solid 185 was automatically assigned to all solids as shown in the last picture below.

[MickMack]

Could you assist me with changing the KEYOPT as described above.
Thanks Michael

[MickMack]

Hi guys Can anyone offer sum advice on how to change KEYOPT2 as detailed above.

Any advice much appreciated

Thanks

[peteroznewman]

The default element order is quadratic, not linear. Therefore the elements that were used were probably SOLID186 and not SOLID185. SOLID186 are quadratic elements and there is no Keyopt(2)=3 defined for this element.
Go to the Mesh Details window and set the Element Order to Linear instead of Program Controlled. Then you will get SOLID185 elements and the command object will work.

[MickMack]

I have already changed the mesh element order to 'linear' and i have checked that the solids are SOLID185, please see both snippets below.

Can i take it that the command snippet below is correct.
et,matid,185
keyopt,_sid,2,3

If so should the snippet be inserted into the tree with the boundary conditions, or do i need to add it to each solid in the geometry tree?
Thanks Michael

[Emperor]

you have to add the extract to each solid in the geometry tree. If you want to use the keyopt on the same element, you must also put matid and not _sid (as far as I know) i.e. :

Et,matid,solid185
keyopt,matid,2,3 ! Simplified enhanced strain formulation

You can then check in the output of the solver that the solid185 has been used with the right keyopt, just do a Ctrl+F and search for "solid185".

[MickMack]

Thanks for the reply
I have added that command to all the solids within my geometry, but it still does not appear to have worked. As you can see the solver is still assigning KEYOPT2(2). 2 images shown below.

I don't see the command snippet in the solver output so i don't believe it is reading it at all. I would expect to see *****Begin Command Snippet* **** in the output file.

I'd appreciate any further suggestions on how to remedy this.

Thanks Michael

[peteroznewman]

you have to set the Element Control to Manual to stop the solver from overwriting your Keyopts.
Under the body you want to apply the control, you insert a command object and type
keyopt,matid,2,3
You don't need the first line because the elements are already type 185.
Regards Peter

[MickMack]

I did what you suggested but i am sorry to say that it is still not working. I have included the images below. I am applying it to all solids in the model.
Michael

[peteroznewman]

What do you mean it's not working?
Before the solver said keyop(2)=2 is suggested and has been reset.
Now it just says keyop(2)=2 is suggested but does not say it has been reset.

[MickMack]

Apologies i did not register that difference,does that mean it is working?

Is there a way to check what keyopts are being used in an analysis? Usually there is a line of zeros beneath the respective keyopts, or a number under it as shown in the previous image.

Thank you for reverting back

[peteroznewman]

Yes, it should show the line of zeros and there will be a 3 in column 2 of the line of zeros.

[MickMack]

I have tested two scenarios both with the element control setting set to 'Manual'. The first on the left in the image below includes the keyopt command (keyopt,matid,2,3 !Simplified enhanced strain formulation) on all the solids, excluding the bolts. The second scenario does not include this command snippet. As shown in the image below both scenarios will "Give Suggestions Only", and i cannot tell what keyopt is active as the customary line of zeros is not shown anywhere in the output file, it seems to only be shown when the setting is "GIVE SUGGESTIONS AND RESET THE KEY OPTIONS",as highlighted in the last image.
I have also been unable to locate the snippet command in the output file, i assume it should be visible in the document.

At the moment i cannot tell if the inclusion of the command is changing the keyopt correctly, as the results appear to be the same even when the command is not included.
Thanks.
Michael

[MickMack]

I have been able to confirm that the keyopts are working correctly by using the command ETLIST,all. In the solution information all the keyopts are visible shown in the last image below.

Thank you again for your generous assistance.
Regards Michael