Force constraint Direction by vector in .inp file?

About the development of the FEM module/workbench.

Moderator: bernd

eggy
Posts: 31
Joined: Thu Jul 30, 2015 12:56 pm

Force constraint Direction by vector in .inp file?

Postby eggy » Sat Jun 24, 2017 3:56 pm

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
User avatar
sgrogan
Posts: 5419
Joined: Wed Oct 22, 2014 5:02 pm

Re: Force constraint Direction by vector in .inp file?

Postby sgrogan » Sat Jun 24, 2017 4:31 pm

eggy wrote:
Sat Jun 24, 2017 3:56 pm
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.
eggy wrote:
Sat Jun 24, 2017 3:56 pm
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
Posts: 31
Joined: Thu Jul 30, 2015 12:56 pm

Re: Force constraint Direction by vector in .inp file?

Postby eggy » Sun Jun 25, 2017 5:19 am

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.
User avatar
bernd
Posts: 8438
Joined: Sun Sep 08, 2013 8:07 pm
Location: Zürich, Switzerland

Re: Force constraint Direction by vector in .inp file?

Postby bernd » Sun Jun 25, 2017 12:02 pm

btw. I like the Part -> primetives -> line tool more for this kind of line
User avatar
bernd
Posts: 8438
Joined: Sun Sep 08, 2013 8:07 pm
Location: Zürich, Switzerland

Re: Force constraint Direction by vector in .inp file?

Postby bernd » Sun Jun 25, 2017 12:09 pm

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.
User avatar
bernd
Posts: 8438
Joined: Sun Sep 08, 2013 8:07 pm
Location: Zürich, Switzerland

Re: Force constraint Direction by vector in .inp file?

Postby bernd » Sun Jun 25, 2017 12:13 pm

for the second question, I do not understand what you would like to do?
UR_
Posts: 991
Joined: Tue Jan 03, 2017 8:42 pm

Re: Force constraint Direction by vector in .inp file?

Postby UR_ » Sun Jun 25, 2017 6:15 pm

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
ScreenshotCaseUnderPointLoad.png (124.94 KiB) Viewed 1633 times

file for testing
CasingUnderPointLoad.FCStd
(141.13 KiB) Downloaded 38 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
Posts: 31
Joined: Thu Jul 30, 2015 12:56 pm

Re: Force constraint Direction by vector in .inp file?

Postby eggy » Mon Jun 26, 2017 10:15 pm

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
User avatar
bernd
Posts: 8438
Joined: Sun Sep 08, 2013 8:07 pm
Location: Zürich, Switzerland

Re: Force constraint Direction by vector in .inp file?

Postby bernd » Tue Jun 27, 2017 5:49 am

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 40 times

screen.jpg
screen.jpg (220.38 KiB) Viewed 1591 times
screen1.jpg
screen1.jpg (101.68 KiB) Viewed 1591 times
UR_
Posts: 991
Joined: Tue Jan 03, 2017 8:42 pm

Re: Force constraint Direction by vector in .inp file?

Postby UR_ » Sun Jul 02, 2017 7:17 pm

bernd wrote:
Sun Jun 25, 2017 12:13 pm
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
SpotWeldedPlates.png (42.33 KiB) Viewed 1539 times
SectionView.png
SectionView.png (14.94 KiB) Viewed 1539 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
inp file modification.png (22.08 KiB) Viewed 1539 times

And this is result view: (color range mapped 0 to 50 MPa)
TieContactVanMises.png
TieContactVanMises.png (234.26 KiB) Viewed 1539 times

file:
TiedSurfaceStripped.FCStd
(23.88 KiB) Downloaded 57 times

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