How implement in prepomax boundary condition - simple support (1 dof at angle 7 degrees ) as in attached photo
thanks in advance for responce
You should define a boundary condition in a local coordinate system. This is not supported in PrePoMax but you can use the built-in keyword editor and add the *TRANSFORM keyword, as per CalculiX’s documentation: http://www.dhondt.de/ccx_2.19.pdf
when will be supported ? 
Features that can’t be added using Keyword Editor have priority so it might take some time. But meanwhile you can easily define it with keywords without leaving PrePoMax.
Some small handbook for Prepomax with examples is necessary . PDF in prepomax documentation site can be treated as good intro/preface
Apart from user’s manual, there’s also examples manual here: Documentation – PrePoMax
It will be updated in the near future. Currently, YouTube tutorials are the main resource for users. They are published regularly.
You could swap external loads and support reactions. Compute the reaction force required at the support and apply it as a distributed load. Then apply a constraint at the right or left end in vertical direction and see if the reaction matches the load you would have applied there in the original system.
alternatively you can add 1D beam element manually (Edit Calculix Keywords), sloped as the position you drawn.
assign very stiff material properties, the easy ways are modulus elasticity multiplied by one thousands.
to make hinged connection of beam 1D element with shell/solid perimeter holes, you can use *Distributing Coupling with Dcoup3d element.
all above are old classical approach to modeling inclined support.
this method are highly recommended, direct to modeling inclined support properly.
Since you have only one roller support in one direction, you could rotate the whole model for 7° and use a normal Displacement/rotation support. Just be careful to apply the loads at appropriate angles.
But a local coordinate system is probably the best solution.
Could you prepare some short sensible tutorial how to do it ?
It’s relatively simple so maybe this step-by-step description will be sufficient:
- Prepare the model normally, including boundary condition that will later be turned into an inclined support. It will be easier if you use a named node set instead of an internal selection.
- Open the Keyword Editor and add this before the step definition:
*TRANSFORM, NSET=nset_name
x_a, y_a, z_a, x_b, y_b, z_b
where:
- nset_name - name of the node set to which a boundary condition was applied (that’s why I recommend using your own name instead of the default one)
- x_a, y_a, z_a - global coordinates of a point lying on the X axis of the local coordinate system being defined
- x_b, y_b, z_b - global coordinates of a point lying in the XY plane (but not on the X axis) of the local coordinate system being defined
That’s it, the only difficulty is specifying proper coordinates of these two points depending on the position and orientation of your model. To make it easier, you can find the coordinates of the center of the local CSYS by creating a reference point using “Center of gravity” method and node set created before. Then imagine how this local CSYS should look like and specify the coordinates of the two points described above.
Just keep in mind that the boundary condition must be applied to proper directions of the local (not global) coordinate system. So again, you have to imagine how this CSYS will look like and which axis will point in which direction.
may implementation is required and could be useful features. also, frequently used in defining concentrate load (specific angles) at ref. nodes. currently user need to input manually in each direction, PrePoMax only checked it’s resultant forces.
Where to find internal Keyword editor in prepomax rest is clear for me which file how to paste it to current model ?
You can find it here: Model → Edit CalculiX Keywords
There expand proper branches of the tree and add new keyword using “Edit selected keyword” field.
Remove those x, y and z letters. There should be only coordinates instead of them.
Where to find complete list of functionalities which can be implemented by keywordeditor in prepomax with sensible examples/tutorials ?
Prepomax software is very good but when crucial functions will be available only by programming-keyword editor then this software will be used only by enthusiast
Best regards
CalculiX offers a wide range of features and it would take a lot of time to implement all of them. The syntax of keywords is very intuitive and CalculiX’s documentation describes all the details (chapter 7. Input deck format): http://www.dhondt.de/ccx_2.20.pdf
It’s just necessary to practice a bit and gain some experience with keyword handling. It’s definitely worth it if you want to give CalculiX a try.
Even in Abaqus some important functionalities, such as imperfections for postbuckling analyses, still have to be added using keyword editor.
The *Transform keyword is useful but only in specific cases, most analyses don’t need it. And if it’s necessary, you just have to add two lines of code with coordinates that you would have to enter manually anyway. Believe me that this is an extremely user-friendly solution when compared with most of the other FEA codes. This is one of the main advantages of CalculiX.
Advanced FEA is never easy, you always have to dive deep into the syntax of the solve’s input files and study the documentation if you want to make full use of professional FEA programs.
And @Michal do not forget, this is open-source software. It is developed mostly as a hobby for the last 5-6 years, while the solver behind it is being developed for 25-30 years. So the user interface will always be behind the solver in terms of supported features.
2 Likes
right @Michal this is commonly use in another FE software. notify as node/element local coordinate system with subscript (x,y,z or 1,2,3) can be useful to defining and displaying:
- inclined support (constraint) and loads at specific angles
- material directions (anisotropic)
- beam axes rotation
- layer fiber orientation (composite)
- results value and plot (e.g ring/curved plate/beam, skew, beam forces/stress in normal directions)
however, as mention by @Matej many solver features is not yet implemented for some reasons. you may trace the history at each versions, also in YouTube channels. it seems the developer respecting user feedback so make it look great at every release.
an example is in contact, plasticity, mesh refinement, shell element, etc. so many implemented features are based on user feedback and the developer interest. it’s okay for me when the features not yet available, still can use keyword editor.