Altair RISE

A program to recognize and reward our most engaged community members

Nominate Yourself Now!

Bolt Pretension effect to the subsequent loadsteps

Altair Forum User

Hi All,

Hope you can post a reply for the query below :

Considering a model ( two plates with a bolt ):

note: the bolt is modelled by Linear elements, i.e, rigid spiders(RB2) at the head and nut end, with 3 beam elements

between them.

I could induce pretension in the bolt by the following ways:

1. applying temperature at the extreme nodes of the bolt,i.e, the independent node of the rb2,

where the one node of beam element and rigid meet.

2. through multipoint constraints.

3. by Gap elements.

But, how would I carry over this pretension effect to the subsequent loadsteps,

where I could use the strain created in the pretension step as the stressed bolt, where I would apply the service load to the model

In simple, how would I 'Lock/Carry' this pretension effect created to the other loadsteps??

NOTE: I'm TRYING TO USE INERTIAL RELIEF TO CALCULATE THE STRESSES IN THE MODEL,in the following loadsteps.

hence I cant use constraints to lock those nodes.

Further , I have also made use of the option CNTNLSUB to carry the bolt strain results forward, but in vain.

Find more posts tagged with

English

Radioss

Accepted answers

All comments

Altair Forum User

Hi,

i can't give a common answer. But for a normal static solution the best way is to use the STATSUB(PRELOAD) command. Please look at the help files.

You can define loadcase 1 and in loadcase 2 you can include the loadcase 1 as PRELOAD.

I don't know if it works for all solution sequences, especially NLSTAT or NLGEOM.

Regards,

Mario

PS: The solver has a new pretension option (described in the help file), but it seems Hypermesh doesn't support the commands at this time. But you can modify the *.fem file of course....

Altair Forum User

Hey Mario,

Firstly Thank you for the reply.

Yeah the options STATSUB(PRELOAD) & STATSUB(PRETEN) & STATSUB(BUCKLING)

were introduced recently to v11.0 by patch.

But these options are available for Linear-Static Analysis.

The reason I cant use the option is because,

there are contacts defined in the model, 8 pairs to be preciese.

And so this option is not valid for NLGEOM or NLSTAT,

neither can I change the Analysis option to NLSTAT from STATIC in linear-static analsyis.

But did try using the NLSTAT, it didn work.

And I aplologize for not informing the same in my post above, thought it would be cumbersome. /emoticons/default_tongue.png' alt=':P' srcset='/emoticons/tongue@2x.png 2x' width='20' height='20'>

but yeah I had modelled two loadcases.

Altair Forum User

In V11, PRETENSION is available by activating subcase-unsupported cards in the load step options.

EDIT the load step and select the SUBCASE_UNSUPPORTED

Go up to the new added definition and in the text box enter: 'PRETENSION = 10' 10 is just a number larger than the largest load step identifier.

Now is the tedious part. Export your .fem deck and open it up for editing.

At the bottom of the Bulk Data section, insert the following:

PRETENS 8 1375141

PTFORCE 9 8 30000.0

8 is another identifier greater than any load step number, 1375141 is the element number of the 1D element you want to pretension.

PTFORCE is the pretension force that applies it to PRETENS which creates the PRETENSION subcase.

For subsequent load steps (sub cases), I haven't found a way to carry the pretensioned element except for including the PRETENSION is each following sub case. In a non-linear solution of NLSTAT or NLGOEM, one can select CNTNLSUB when editing the load step to add a preceding load step set of results to the present load step.

V12 is supposed to have better subpanel selections to create pre-tension but I haven't found it yet in a beta version I am running.

Also, if you contact hwsupport@altair.com, you should get a reasonably quick response and get the help you need. I find them most helpful.