Hi,
I would like to create a set similar to the one below.
Using the findAt method is time consuming because it would require to enter the coordinates of all the edges that I need.
Instead, using the getByBoundingBox method, I can get all the edges lying inside a box without struggling to find the exact coordinates.
The issue is that I would like to exclude certain entities from the "BoundigBox". So I'm looking for the method equivalent to pressing Ctrl to unselect entities in th GUI. When I record a macro or through the journal file there is no such a method. Instead, when I use Ctrl to unselect entities, an new set (in this case) is created.
Does anyone know of a built-in Abaqus python method to reproduce the unselect operation?
Otherwise, does anyone have any suggestions for an efficient way to add entities to python scripts without using the findAt method? It gets messy when dealing with many entities, and specially if one needs to parametrise the code...
Thank you,
Sérgio
In python, a set of edges behaves like any regular list (of edge objects), so you can add and subtract among lists using standard python functions. this allows you to easily remove from a set the edges you want to "unselect".
As to how to find edges without using findAt, it's sadly up to your imagination and finding clever ways to leverage the information you can get from your model. Try to use all the available methods and members of an Edge object to see if there's a better way to identify a particular edge. As an example, below is a script that finds horizontal and vertical edges of a part and create two separate lists.
> part = mdb.models['Model-1'].parts['Part-1']
> horizontal = ()
> vertical = ()
> for counter in part.edges[:]:
> id = counter.index
> a = counter.getVertices()
> p1 = part.vertices[a[0]].pointOn[0]
> p2 = part.vertices[a[1]].pointOn[0]
> if p1[0] == p2[0]: # part.edges[id] is along X axis
> horizontal+=part.edges.findAt(part.edges[id].pointOn[0]),
> elif p1[1] == p2[1]: # part.edges[id] is along Y axis
> vertical+=part.edges.findAt(part.edges[id].pointOn[0]),
it might not be the prettiest code, but it gets the job done.
Also be careful that when you add calculations to an if-clause, python may fail to find edges (i suspect this comes from rounding errors on floats). From previous example, say you want to find edges of length 3 along X-axis, instead of doing this, which seems logical:
if abs(p1[0] - p2[0]) == 3: # this may fail to find all occurrences
use instead:
if abs(p1[0] - p2[0]) - 3 < 1.e-5: # this works.
As you can see, these are useful if you need to find lots of edges, but for few occurrences, findAt still remains the easiest method.
hope this helps.
Hi Sérgio Costa,
If I want to explain it in detail, it could take a while, and it has a long explanation. Refer to the link below. There, you will see an example that can help you resolve your problem.
https://caeassistant.com/product/python-scripting-in-abaqus-part-2/
I hope you can get it done.
Best luck, friend.
Martin Veidt your answer looks like spam as it is. Could you be more specific? Which example are you talking about?
Hi Sérgio,
As previously suggested, you can combine mutiple functions such as "findAt" or "getByBounding..." and perform whatever checks and combinations you need.
However, in this particular case I would findAt the front face of your model and then select all the edges that make this face.
I recommend the following video explaining multiple ways to select geometry using these and other functions: https://youtu.be/AYt_4QgXv3I
By the way, to create the set you cannot use a LIST of edges, but an EdgeArray (which is very similar, but Abaqus will complain otherwise).
Best regards Sérgio!!
You are right that this selection stuff can be quite tedious in Abaqus/Python scripts.
In this case, I would first create a set of all edges on the left side and a set of the edges to be excluded using "findAt" and/or "getByBoundingBox". And then use "SetByBoolean()" to create a set of the difference of those two sets. Selecting the edges by their size would also work in this case.
I teach a course on scripting Abaqus CAE using Python and there the main part is how to select cells, faces, etc. You can find my introduction into this here: https://www.martinpletz.com/fe-scripting-3/ and I made a small cheatsheet for Abaqus/Python commands that you can find there: https://github.com/Marple85/lv_abq_python_2021/raw/main/Cheatsheet-ABAQUS-Python_en_v2.pdf
(yes, this is shameless advertisement, but since it's all free I hope you don't mind)
Cheers, Martin
- Badges
- Science topic