turn on suggestions

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

Showing results for

- Navigation
- Simcenter
- Forums
- Blogs
- Knowledge Bases

- Siemens PLM Community
- Simcenter
- 3D Simulation - Femap Forum
- modal Random response stresses.

Options

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

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

07-29-2015 03:23 PM

**resubmitted with Random spelled correctly....**

** Can anyone give a clear recommendation on the easiest way to get stress out of the Femap random, modal solution? The Femap doc's don't cover it as far as I see and references to it are rather convoluted. Seems like the SPCD card needs 386.4 factor when requesting stresses. Is this implementable in Femap or does the card have to be edited manually?**

** Infinite mass doesn't seem to run so we switched to nodal enforced displacement/acceleration and direct solution. A modal frequency table is being used. all other functions related to this are a constant 1.0, except of course the PSD stimulus function which is defined in log-lot G^2/Hz.**

** I guess the trick is to get all these inputs consistent somehow.**

**RLOAD2,10,11,,,12,,ACCE**

**SPCD,11,2,386.4**

Solved! Go to Solution.

16 REPLIES

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

07-30-2015 10:51 AM

See example 18 "Random Response of Hinge Model" in the Femap examples under Help. It covers both large mass and "SPCD" methods for random response as well as some notes on making consistant inputs.

Regards,

Joe

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

07-30-2015 11:03 AM

I've seen all the examples and tutorials. None of them have comprehensive coverage. Only special examples, without stress recovery (scaling/units question). We;ve used that as a guide. Unfortunately it didn't work.

Could you provide an example .dat file for stress recovery? The example also has pre-made files on hand.....not starting from scratch.

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

07-30-2015 11:24 AM

To request stress output for random response, do the following:

Use the "all" radio button as shown below

Now under Analysis Manager; Output Requests, select "stress"

This will write the following Case control in your Nastran deck:

STRESS(SORT1,PLOT,NORPRINT,PHASE,CORNER,RALL) = ALL

Now the op2 file will contain the RMS stress output for all applicable elements.

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

07-30-2015 12:03 PM

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

07-30-2015 02:46 PM

I think I see the source of your confusion, and the example is not consistent.

In the example, the PSD is given in g^2/Hz; therefore the unit acceleration load should be entered as 386.14in^2/sec since the model units are inches. This input will give correct units for all output(including stresses). However, when you look at acceleration output, remember that it is now in (in/sec)^2. So if you are looking at the base drive location, and want to see that the input and output are equivalent, then you will need to scale the accel back to g^2/hz. This means multiply the accel by 1/((386.14)^2) You can apply this scale factor to your data series to make the input and output charts have the same units.

So to try to summarize consistent input:

if PSD is given in g^2/Hz, the unit accel excitation should be the value of g(in your proper units)

if PSD is given in (accel units)^2/Hz, then the unit accel excitation should be a value of 1.0

We will try to update the example to be consistent and include the new Case Control options for requesting output

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

07-30-2015 04:15 PM

Thank you. Seems like if you are looking at accelerations you run it one way, If you're looking for stresses run it the other way.

The example of the large mass method uses a Mass/Accel Scale Factor of 0.0070248 (page 18-8 V11.1). The reciprocal is 142.37. What does this correlate to? Does't seem to be a multiple of 386.4 or 9.8.

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

07-30-2015 04:39 PM

My advice would be to always use consistent units for input. Then you can always scale or transform results to make them easier to understand after the analysis run. You just need to make sure you understand the units and orientations of input and output. I'm sorry the example violates this advice.

We also suggest using the "direct" or SPCD method for enforced motion.

The large mass method is still supported does still work, but it is sort of old technology. Notice you are actually defining a force, not an acceleration directly as in the other method. The large mass method requires you to scale the force along with the large mass so the resulting input is a proper acceleration of the drive location.You are using this "trick" to input an acceleration that is defined by F=Ma. You can find many references online about details of the large mass method of enforced motion.

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

08-05-2015 09:38 AM

Tried those settings. VM stresses ranged from 0 to 1.

Load is acceleration on node 386.4, rbe'd to the rest of the structure.

Load factor is 1.0 across the frequency range.

.dat lines:

SOL SEMFREQ

TIME 10000

CEND

TITLE = Random Response Vertical - Main Housing

ECHO = NONE

DISPLACEMENT(SORT2,PLOT,NORPRINT,PHASE,RMS) = ALL

ACCELERATION(SORT2,PLOT,NORPRINT,PHASE,RMS) = ALL

SPCFORCE(SORT2,PLOT,NORPRINT,PHASE,RMS) = ALL

OLOAD(SORT2,PLOT,NORPRINT,PHASE,RMS) = ALL

GPFORCE(SORT2,PLOT,NORPRINT,PHASE) = ALL

FORCE(SORT2,PLOT,NORPRINT,PHASE,CORNER,RMS) = ALL

STRESS(SORT2,PLOT,NORPRINT,PHASE,CORNER,RMS) = ALL

SPC = 5

BGSET = 114

FREQUENCY = 1

METHOD = 1

SDAMPING = 3

RANDOM = 200

SUBCASE 1

DLOAD = 7

BEGIN BULK

PARAM,POST,-1

PARAM,OGEOM,NO

PARAM,AUTOSPC,YES

PARAM,GRDPNT,0

RANDPS 200 1 1 1. 0. 4

$ Femap with NX Nastran Function 4 : PSD Input

TABRND1 4 LOG LOG +

+ 8.647006.03967889.127396.03662569.607785.03396999.665451.0336723+

.

.etc. (remainder of psd function)

+ ENDT

CORD2C 1 0 0. 0. 0. 0. 0. 1.+FEMAPC1

+FEMAPC1 1. 0. 1.

CORD2S 2 0 0. 0. 0. 0. 0. 1.+FEMAPC2

+FEMAPC2 1. 0. 1.

PARAM,RPOSTS1,1

$ Femap with NX Nastran Function 3 : Damping 0.05 vs Freq

TABDMP1 3 CRIT +

+ 8. .05 120. .05ENDT

PARAM,LFREQ,8.

PARAM,HFREQ,110.

EIGRL 1 110. 0 MASS

$ Femap with NX Nastran Load Set 7 : random Vibe

$ Femap with NX Nastran Function 1 : LF 1.0

TABLED2 1 0. +

+ 8. 1. 120. 1.ENDT

RLOAD2 101 102 1 ACCE

SPCD 102 15 2 386.4

DLOAD 7 1. 1. 101

FREQ 114.6418215.4552516.2686817.0821217.8955521.9955823.21755+

+ 24.4395325.6615126.8834831.5539233.01127 33.086633.3069133.86624+

+

.

.etc. (remainder of modal frequency table)

$ Femap with NX Nastran Constraint Set 5 : fixed on input node

SPC1 5 123456 15

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

08-05-2015 09:39 AM

Follow Siemens PLM Software

© 2018 Siemens Product Lifecycle Management Software Inc