Turn on suggestions

Auto-suggest helps you quickly narrow down your search results by suggesting possible matches as you type.

Showing results for

Auto-suggest helps you quickly narrow down your search results by suggesting possible matches as you type.

Showing results for

** Community Tip** - Have a PTC product question you need answered fast? Chances are someone has asked it before. Learn about the community search.
X

- Community
- Creo+ and Creo Parametric
- Analysis
- Re: Understand which parameters can be extracted f...

Options

- Subscribe to RSS Feed
- Mark Topic as New
- Mark Topic as Read
- Float this Topic for Current User
- Bookmark
- Subscribe
- Mute
- Printer Friendly Page

Aug 29, 2018
07:12 AM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

Aug 29, 2018
07:12 AM

Understand which parameters can be extracted from Flow Analysis

Currently we are running some external CFD analysis on parts of our robot to get the lift and drag coefficient and the center of pressure [1].

The simulations are performed using ANSYS Fluent [2].

Considering that the CAD model of the robot is designed using PTC Creo, and considering that recently PTC has introduced a module for flow analysis [3], we would like to run such simulations directly in Creo.

The only problem is that so far we didn't find a document or a video explaining how to get the lift and drag coefficient and the center of pressure.

Here the questions:

- Do you know if it is possible to get the lift and drag coefficient and the center of pressure for external CFD?

- Do you have a link to a document that explains how to run such simulations?

- Which package (basic, plus or premium) should we buy?

Thank you.

[1]:https://www.youtube.com/watch?v=jNnQeKuF7PI

[2]:https://www.ansys.com/it-it/products/fluids/ansys-fluent

[3]:https://www.ptc.com/-/media/Files/PDFs/CAD/Creo-5/Datasheet-Creo_Flow_Analysis-en.pdf

Streamlines for a flow around the iCub head with Re=4x10^5 (velocity= 15 m/s). Simulations with Ansys FLUENT. Post-processing with CFD post inside FLUENT. Locomotion and Control IIT

20 REPLIES 20

Aug 30, 2018
05:35 AM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

Aug 30, 2018
05:35 AM

Sep 07, 2018
03:05 PM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

Sep 07, 2018
03:05 PM

Hi,

Yes, you can select the surface and create a xyplot to monitor pressure or shear force on that surface.

To compute lift and drag coefficient, we can use expression to do that very easily. You can use expression to define equations and formula. We also support user defined variable for xyplot.

Example of cl, cd calculation

-----------------------------------------------

den=1.16

area=1

aoa=15*pi/180

vmag=200

cx=cos(aoa)

cy=sin(aoa)

nx=-cy

ny=cx

drag=(flow.px@patch.surfname + flow.tx@patch.surfname)*cx

+(flow.py@patch.surfname+flow.ty@patch.surfname)*cy

lift=(flow.px@patch.surfname + flow.tx@patch.surfname)*nx

+(flow.py@patch.surfname+flow.ty@patch.surfname)*ny

plot.cd = drag/(0.5*den*vmag^2*area)

#plot.cd: Drag Coefficient []

plot.cl = lift/(0.5*den*vmag^2*area)

#plot.cl: Lift Coefficient []

-----------------------------------------------------

here flow.px@surfname means pressure force x component from flow module at surfname patch

similarly, flow.tx means shear force x component.

For the center of pressure, we need to do an integration of x times pressure of x component on all external surfaces and it is straightforward to use expression to write it.

----------------------------------------------------------------------

cpx = integral(x*flow.pressure*normal.x, patch.surfname)/flow.px@surfname

plot.cpx = cpx

#plot.cpx: Center of Pressure x []

----------------------------------------------------------------------------

Please contact me if you got further questions!

ls@simerics.com

Thanks.

Sep 07, 2018
04:43 PM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

Sep 07, 2018
04:43 PM

Hi

For the package, if you only have external fluid dynamics problems. You only need the basic package, that includes flow, turbulence, heat transfer and all post processing tools. The setup is very straightforward. Most of external fluid problems, we can get the converged solution in couple minutes. We can also show the results in the real time during the calculation.

For the cl, cd and center of pressure calculation, you can select the surface and create a xyplot to monitor pressure or shear force on that surface.

To compute lift and drag coefficient, we can use expression to do that very easily. You can use expression to define equations and formula. We also support user defined variable for xyplot.

Example of cl, cd calculation

-----------------------------------------------

den=1.16

area=1

aoa=15*pi/180

vmag=200

cx=cos(aoa)

cy=sin(aoa)

nx=-cy

ny=cx

drag=(flow.px@patch.surfname + flow.tx@patch.surfname)*cx

+(flow.py@patch.surfname+flow.ty@patch.surfname)*cy

lift=(flow.px@patch.surfname + flow.tx@patch.surfname)*nx

+(flow.py@patch.surfname+flow.ty@patch.surfname)*ny

plot.cd = drag/(0.5*den*vmag^2*area)

#plot.cd: Drag Coefficient []

plot.cl = lift/(0.5*den*vmag^2*area)

#plot.cl: Lift Coefficient []

-----------------------------------------------------

here flow.px@surfname means pressure force x component from flow module at surfname patch

similarly, flow.tx means shear force x component.

For the center of pressure, we need to do an integration of x times pressure of x component on all external surfaces and it is straightforward to use expression to write it.

----------------------------------------------------------------------

cpx = integral(x*flow.pressure*normal.x, patch.surfname)/flow.px@surfname

plot.cpx = cpx

#plot.cpx: Center of Pressure x []

----------------------------------------------------------------------------

Please contact me if you got further questions!

Thanks.

Dec 10, 2018
04:08 AM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

Dec 10, 2018
04:08 AM

amazing

May 27, 2020
02:58 AM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

May 27, 2020
02:58 AM

Hello CFD Geek,

I really want to know the drag coefficiënt of a car I developed. (it's for school en for the shell ecomarathon) Could you help me? I have no clue what I need to do...

I put the body into flow analysis and everything works, I just don't understand what I need to do to get the drag coefficiënt...

Please help 🙂

May 28, 2020
03:04 PM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

May 28, 2020
03:04 PM

Hi Ruben1,

It is very simple to do that in Creo Flow. We have a tutorial for external flow to demonstrate that. I will send you the link soon. Thanks.

May 29, 2020
04:07 AM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

May 29, 2020
04:07 AM

Thanks! I could really use that tutorial!

I don't wanna be rude, but I need to hand in my paper in 3 weeks, would be nice if I can put the result in my paper...

Thanks again!

Ruben

May 29, 2020
02:33 PM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

May 30, 2020
05:41 AM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

May 30, 2020
05:41 AM

1. In the Flow Analysis Tree, under Physics, select Common.

2. Click :

XYPlot. A new entity xyplot3 is added in the Flow Analysis Tree under Results > Derived Surfaces > XY Plots.

This plot doesn't show up for me tho...

Jun 01, 2020
07:20 AM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

Jun 01, 2020
11:50 AM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

Jun 01, 2020
11:50 AM

Hi, if that does not show up, it means you are using some old version of creo parametric. What version are you using? Please make sure you are using the same version as in that tutorial. If you cannot upgrade creo parametric, that custom variable is saved in a file called xxx_integrals.dat in the folder of your creo model. You can find it out from that file after the simulation finished.

Jun 02, 2020
03:44 AM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

Jun 02, 2020
06:00 AM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

Jun 02, 2020
06:00 AM

The 2nd column is your cd, please refer the column data to its caption title

Jun 02, 2020
06:06 AM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

Jun 02, 2020
06:06 AM

Hi,

Do you mind mentioning which school team are you working for this project? We may help your team on that project for CFD and aerodynamics design questions. thanks.

Jun 03, 2020
09:54 AM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

Jun 03, 2020
09:54 AM

hello cfdgeek,

We are from 'Vives Kortrijk - Belgium.'

"The 2nd column is your cd, please refer the column data to its caption title"

How do I need to do that exactly?

I uploaded the xxx_integrals.txt 🙂

Jun 04, 2020
03:12 PM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

Jun 04, 2020
03:12 PM

That is the drag coef you are look for.

Jun 04, 2020
03:14 PM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

Jun 04, 2020
03:14 PM

`time userdef.Coefficient_of_Drag`

the 2nd column data

Jun 04, 2020
04:23 PM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

Jun 04, 2020
04:23 PM

yes, but there are so many different values in that 2nd column data. wich value is the right one?

Jun 08, 2020
03:31 AM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

Jun 08, 2020
03:31 AM

??

Jun 08, 2020
03:49 AM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Notify Moderator

Jun 08, 2020
03:49 AM

For sure you get a list of CD, CFD solves the NS equations iteratively. Your CD should converge to the true CD while you residual get converged. Just take the value when the solution get converged.