I want to send an inventor model to Mechanical Simulation, define the loads there but I’d like to calculate the loads’ values in an external program (I use ilogic) and read them in Mechanical Simulation.
The first thing I tried was to define the loads in Inventor Stress analysis environment but then I cannot update the Mechanical Simulation model (it only overwrites or asks for new file name)
The second option was to use “Load curve” with a constant value but it’s only available in nonlinear analysis and I think I have to load manually each time
It would be nice if Mechanical Simulation loads would be able to read the inventor parameters that are transferred.
Thanks in advance
I'll try to explain why it would be nice to read load values from outside Mechanical Simulation automatically.
My customer is using a product configurator made with ilogic in Inventor.
Now they would like to analyze the design (the part is always the same, only dimensions change).
The loads applied to the design are always the same, only change the value and the position
To calculate the values of loads we use a set of equations that uses input from user and some geometrical dimensions from the part.
It's easier to make this calculation of load values outside Mechanical Simulation. I know there are formulae in MS but I don't see how to use a Inventor parameter (part dimension) as input.
So, the need is to make it easier for the user, who is not an expert in simulation nor MES, he makes around 20 designs/day and he want to design and analyze as fast as possible.
please let me know if you need more information
The command that you are looking for is "Loads from File". (Click the link to go to the Help documentation.) Whether this command will work for you depends on the analysis type, the type of load, and how you know what nodes/elements/faces to load.
Take a look at the documentation and then ask some more questions. What would be helpful to know is:
- analysis type (MES?)
- type of load
- what else?
Simulation Mechanical user since Dec 1997
Thanks for replying.
My analysis is static stress analysis but I changed to "Static Stress with nonlineas materials" in order to being able to use "loads from file".
Its seems that the input file (.xyz) contains forces that are applied to specific nodes.
What I have are pressures (10) applied t specific surfaces. I don't see how can I send he values I read to the values of pressures already created.
The easier way I've found to do it is to define the loads in Inventor but the problem is I have to recreate the .fem file each time I modify something and I wil to do some configuration each time: define element, some boundary conditions...anyway I think I would have more work defining the values of the loads.
Let me give you my ideas before I reply to you comments.
(1) My idea is to apply a dummy pressure (like 3.14, 999) to the faces where you want to apply your pressure. Then use iLogic to replace the dummy pressure with your value. It will take some work because the information is in multiple files, but here are the general steps:
- Create the model with the dummy loads.
- Do a Check Model ("Analysis > Analysis > Check Model")
- Your program reads the file ELEMCOND.dbf and locates the elements that have the dummy load applied.
- Your program reads the file ELEMENTS.dbf to find out which nodes are on the face of that element.
- Your program reads the file NODES.dbf to get the coordinates of the nodes on the face of the element.
- Your program calculates the pressure based on the position, etc, and overwrites the dummy pressure in ELEMCOND.dbf.
The .dbf files are Foxpro database files which I think iLogic will be able to read directly.
(2) Let's pretend the name of the Inventor file is MyModel. You transfer MyModel to Simulation Mechanical, apply all of the loads, constraints, etc. When the model is ready to be analyzed, do a "File > Save As" and call it "MyModel variation A". You then change MyModel in Inventor and transfer it to Simulation. The associativity should keep all of the input (except for nodal loads) because "MyModel" is ready to be analyzed (just like MyModel variation A). Make any additional changes needed and do a "File > Save As" and call it "MyModel variation B". Repeat changing "MyModel" and saving it as "MyModel variation X".
Now, a couple of comments on your last post.
- Linear Static Stress should be able to read loads from a file: "Setup > Loads > Loads from File". You should not need to use Nonlinear Static Stress.
- Any type of load that can be applied through the interface can be read from a text file. Nodal loads are easier because the coordinates of the nodes are relatively easy to get. (Use the "Results Inquire > Inquire > Current Results" to get those.)
Have fun. I have some programs that I have written in VB6 that may be a good starting point.
Simulation Mechanical user since Dec 1997