Force constraint Direction by vector in .inp file?

[eggy]

I need to place a Direction on the force constraint on my model. It is placed on the inside of the cylindrical face. I want to choose a Direction that does not match any face or edge in my model.
Is it possible to edit the .inp file (is that where I would find the Direction?) or other file to put in a vector?
I use Paraview quite successfully with the FEM Workbench, and this is one of two limits for me right now.
Also, can circle constraints function for bolt holes over a token-sized area like in ANSYS?

Thank you for an alternative for somebody to learn from without expensive programs or trials!

Eggy

[sgrogan]

I need to place a Direction on the force constraint on my model. It is placed on the inside of the cylindrical face. I want to choose a Direction that does not match any face or edge in my model.

Use the Draft WB to draw a line. This line can then be used as a direction vector.

Also, can circle constraints function for bolt holes over a token-sized area like in ANSYS?

I don't understand this part. Could you elaborate?

[eggy]

Thank you, I'll try the Draft WB to create an edge to pick as my Direction vector. Is is in the .inp file anyway? Or Direction only takes a face or edge as a Direction vector?

My second part was how to properly model the two bolt holes I have on my bracket. I would normally make them similar to an annulus area to model the bolts clamping pressure under the head/washer in ANSYS.

[bernd]

btw. I like the Part -> primetives -> line tool more for this kind of line

[bernd]

the constraint pressure uses dload in ccx and thus uses face normal as direction.

the contraint force uses cload and thus the main coordinates system axis. What we do is splitting the user given force with its direction into the main directions. Means no you can not see the force direction vector in the inp file.

But it does not mean it is not possible, to rotate the coordinate system in the inp file. But this would not make sense for FreeCAD in this use case.

[bernd]

for the second question, I do not understand what you would like to do?

[UR_]

Hello eggy,

attached you can find a little example of a cylindrical face with point load applied under arbitrary direction.
Of course some sketches are needed to define direction and hitting spot (in this case by yaw and pitch).
Please note, that geometry used for meshing by gmesh contains:

1. point of load
2. a line, which connects that point to remaining edges (that's because gmsh evaluates his mesh this way: 1D->2D->3D)

ScreenshotCaseUnderPointLoad.png (124.94 KiB) Viewed 1730 times

file for testing

CasingUnderPointLoad.FCStd

(141.13 KiB) Downloaded 41 times

was done with:
OS: Windows 10
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.17.11432 (Git)
Build type: Release
Branch: master
Hash: 0768ae99cfd6036601f66658f6e0f923de9af6f2
Python version: 2.7.8
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 7.1.0
gmesh_3.0.3.exe
ccx_2.12_MTNO.exe

[eggy]

Thanks to bernd and UR_!

All of your help was fruitful in my analysis.

I have another question about applying forces. If I have a tube that is 2.5 m long, and I want to apply 8 point loads, not area loads to it can I do that, or do I have to split the part into 4 sections?

Think of a ride lap bar with 4 people/8 hands pushing laterally on it is what I am after.

Thanks!

eggy

[bernd]

I do not like point loads thus I would make a small face and apply the load to the face, but you could use a vertice and a point load too. Use BooleanFragments to make a union of your pipe a and the vertices. Than you have something to apply your load too. If you mesh this BooleanFragments gmsh creates nodes at each vertices of the shape.

attached my version with a face. In addition I used a MeshRegion to mesh the face with finer elements.

bernd

pipe-pointload.fcstd

(948.52 KiB) Downloaded 43 times

screen.jpg (220.38 KiB) Viewed 1688 times

screen1.jpg (101.68 KiB) Viewed 1688 times

[UR_]

for the second question, I do not understand what you would like to do?

i think eggy is talking about such a feature, which calculix calls a "tied contact"
(e.g. bonding two faces together, even if there is a gap in between)

Below you can find an example containing two not connected plates (gap 0,1 mm).

SpotWeldedPlates.png (42.33 KiB) Viewed 1636 times

SectionView.png (14.94 KiB) Viewed 1636 times

Tie contact was defined by FemConstraintContact (face master and face slave)

Of course ccx's input file needs some modification (but low impact!)

inp file modification.png (22.08 KiB) Viewed 1636 times

And this is result view: (color range mapped 0 to 50 MPa)

TieContactVanMises.png (234.26 KiB) Viewed 1636 times

file:

TiedSurfaceStripped.FCStd

(23.88 KiB) Downloaded 66 times

[rhetorical]
Would this feature be usefull, ... if implemented?
[/rhetorical]