v2.1.11 I get the same message and ignore it
Ok, I thought there was nothing in the 3D view because of that but it updated eventually after switching to the Geometry tab.
The problem with the frequency analysis check here is that contacts are defined between the two halves and would have to be switched to tie constraints to work as expected.
Yeah, I did the same. I got memory errors with the original mesh. Those pins can also be tied to some extent.
Start simple, fail quick !
Am using v2.1.0 - but you guys have lost me with all the other comments.
I thought I did have tie contact between the 2 partsā¦
When I tried tie constraints instead of contacts I got other errors as reported previouslyā¦
This converges.
Then you can introduce the spring and compression only constraints.
This converges too.
Then you can look at replacing the ties with contact.
Thanks Trevor - Iām trying to learn here, can you tell me what was āwrongā?
Ideally Iāll need to repeat with some bolt pre-tension, so I have to make sure I can get things to work hereā¦
top part of die is unconstrained without some interaction with the pins that stop it sliding off.
Advice, feel free to ignore:
- start with linear elements and linear analysis , the job will run quick and you 'll debug faster
- start with ties and look at the reaction between the plates. If the plates are not trying to separate with the bolt preload applied then non-linear contact might be avoided. Look at S33 and set the contours as shown anything in red is trying to seperate and contact would be more better, anything in blue is in compression and therefore in contact.
- add non-linearity ie contact but keep elements 1st order
- finally 2nd order elements put midside nodes on geometry in the mesher and watch the convergence monitor, wait patiently, pray and maybe cry a little.
Donāt think so - the top part and the bolts are a single part (done to simplify things) - the bottom ends of the bolts are fixed, hence the top plate is fixed (apart from any slight flex in the bolts).
Trevor - thanks for taking the time to look at this! Iāve been tearing my hair out.
I really wonder why 2nd order is the default mesh type if it causes such problems! This is a real headache if you arenāt used to having to set mesh type.
Is there any reason why S33 is used in the software rather than SYY (which would be more obvious). Is the relationship of numbers to axes fixed, or can it be edited somewhere?
Iāll start again and see if I can make some progress.
Because first-order tetrahedrons are rarely used for actual calculations, they are very inaccurate and would require huge meshes to provide good results. So they are good pretty much only for initial testing and some dynamic or thermal analyses.
Thatās the convention used also in Abaqus. Normally itās X = 1, Y = 2, Z = 3 but if you use elements having local directions (beam/shell) or a user-defined cylindrical coordinate system then it may not be the case anymore.
this part is fixed, itās not going anywhere solid_part-8
what stops this part solid_part-1 from sliding off
2nd order for stress
1st order need to be used with care
S11, S22, S33, global axes
you can add your own local axes or material axes
Did you use Creo or any other p-element code in the past? Not recommended but you can change the default mesh type under setting ā Meshing ā Mesh type ā Second order Yes/No.
Also itās recommended in the first step to simplify the geometry by supressing small features (if they are not important for the solution) to make the mesh less heavy, espacially by using 2nd order elements (you really should use them for real world problems).
Attached the .pmx file with my suggestions. The mesh is too coarse and distorted, but because of the small chamfers and fillets which i couldnāt suppress, the mesh still ends up with 200000 nodes and needs ~9GB free RAM for the solution with frictional contact. I assume you donāt have a lack in RAM so you can blow up the mesh any further.
good to see the community working overtime 
Just for completeness what does the contour of COPEN look like on the inside
Also I guess if youāre looking for the pretension to properly close the die then as a first pass you can run a coarse mesh like this anyway or 1st order to get close quickly. I reckon the 1st order mesh would take 2 mins. Then get back to 2nd order for the final interation.
Well Iād assumed the Tie would - maybe thatās something else I donāt understand. Iām used to contact conditions with meaningful names - hence easy to set up (though maybe not as versatile)
- Separation, no sliding
- Sliding, no separation
- Separation
- Welded
When trying to use contacts, Iād assumed friction would prevent sliding. How silly of me.
The full design does include some alignment parts which sit in the larger holes around some of the bolts - Iāll put 2 of those back in.
Gunnar - thanks for taking the time. Unfortunately your file doesnāt open for me
Message says it is either corrupted or created in an earlier versionā¦