Learning Forum

[MickMack]

Hi folks,

I have checked some other discussions but i have not been able to find a solution, hence the new post.

Simply i want to be able to select a line of nodes or even a single node within a solid, as shown in the image below i want to select a line of nodes at the centre of the bolt.

[Erik Kostson]

Hi

First of all, only if you have a split edge at the centre will the mesher guaranteed put nodes on that centre line - if there is no edge, then it can not be sure that the nodes will be on that centre line.
Having done the above, then one can select the edge, create a Named Selection - then highlight that named selection right mouse button click on it and choose create nodal named selection (that is shown below, created from Selection).



Another way is to use the worksheet in named selections to choose nodes at a certain location (you could define a local coordi. system there on the edge and use X=0, Y=0,.. to select them in the worksheet).

Hope this helps

Erik

[Vigneswaran Sridharan]

Hi One can select a particular node/nodes from WB GUI and right-click to select the option 'Create Named Selection'.
If the nodes are to be selected from surface/bodies, then create a Named Selection for the particular SUrface/body. Right-click the Named Selection and select 'Create Nodal Named Selection'.
You could try to model the bolts as line body with 'fixed joint' or 'MPC Bonded contact'.
Vigneswaran

[MickMack]

Thanks you both very much for your answers.

I had avoided inserting a cut face as it was causing problems with my multizone hex mesh generation, and i did not want to apply the changes to a single bolt to resolve them. In any case if i have to do this after i have tried the other options i will have no choice.

Again the prompt response is much appreciated.
Cheers Michael

[peteroznewman]

In Mechanical, you can create a Path that runs along the centerline of the bolt. ANSYS will interpolate the stress from the elements that intersect that Path and give you a chart of stress vs Path length.
The Path is created under the Construction Geometry folder.

[MickMack]

Hi
Thank you for your suggestion i will keep this in mind.

By way of an update i am carrying out a different simulation, compression test on a concrete cylinder. I wanted to plot stress vrs strain at regularly spaced nodes along a vertical line on the external surface (long1-11) and at another parralel line within the cylinder (Internal Long 1-11).

To do this i turned on the node numbers and orientated themodel soi could read the node id's. It is not elegant but in this instance it worked.

The alternative options are detailed above particularly creating a local co-ord system and also splitting the solid.
Thanks to everyone for there assistance with this.

Cheers Michael

[MickMack]

Hi
Using the split body and split face features in Spaceclaim is the most effective way to do this. After splitting the body of the cylinder and the faces i added all the solids to a single component, opened the compnent and then used the share command.
This does alter the results from the original single solid body, but in this instance the difference is acceptable.
Please see wireframe of solid below.