Problem with exported Nastran code file

Altair Forum User · January 2015

Hi

I am new to this and just start learning. And I have a problem as following.

The structure I want to analysis attached. It is a truss. I first create four nodes and draw 6 lines. The mesh type is line mesh. I follow all the instructions, but when I wanted to use nastran to solver it, it didn't work and ther warning message was USER WARNING MESSAGE 4698 (DCMPD). I finally managed to get it work by comparing the corrected version of the code to my code. Below is the code that works, but mine has some differences. I found out that it was due the grid points that assigned to SPC and Force. In the corrected version below, the grid points are all from 5 to 8, but my are from 1 to 4. After I change my 1 to 5, 2 to 6, 3 to 7 and 4 to 8, everything worked out and I got the solution. So Anyone know why the ID of the nodes become 5 to 8 but I can still find the nodes by id using 1,2,3, and 4? And how to solve this problem instead of digging into the code file and changing the number? Thanks in advance.

SOL 101

TIME 60.0

CEND

SUBCASE 1

LABEL= static force

SPC = 1

LOAD = 2

DISPLACEMENT(PRINT,PUNCH) = ALL

STRESS(PRINT,PUNCH) = ALL

BEGIN BULK

PARAM,AUTOSPC,YES

PARAM,GRDPNT, -1

PARAM,POST,-1

GRID 1 0.0 0.0 0.0

GRID 2 1000.0 0.0 0.0

GRID 3 1000.0 1000.0 0.0

GRID 4 0.0 1000.0 0.0

GRID 5 0.0 0.0 0.0

GRID 6 1000.0 0.0 0.0

GRID 7 1000.0 1000.0 0.0

GRID 8 0.0 1000.0 0.0

CBEAM 1 1 5 60.0 1.0 0.0

CBEAM 2 1 6 7-1.0 0.0 0.0

CBEAM 3 1 7 80.0 -1.0 0.0

CBEAM 4 1 8 51.0 0.0 0.0

CBEAM 5 1 8 60.7071070.7071070.0

CBEAM 6 1 7 50.707107-0.707110.0

PBEAM 1 1576.0 27648.0 27648.0 0.0 46720.45

MAT1 168950.0 0.33 2.77E-09

FORCE 2 6 01.0 2500.0 0.0 0.0

FORCE 2 6 01.0 0.0 -4330.0 0.0

SPC 1 7 3 0.0

SPC 1 6 3 0.0

SPC 1 8 123 0.0

SPC 1 5 123 0.0

ENDDATA

<?xml version="1.0" encoding="UTF-8"?>

Altair Forum User · January 2015

One another question, I have a solid mesh of the structure as attached. And I applied two 1000N of forces to two nodes when I was assigning the force. But when viewing it in 3D, I saw there were force vectors at each surface layer(see attached picture). So if there are 4 layers(5 surfaces), does it mean that the total force apply to the structure will be 5*2000N = 10000N or it is still 1000N? Thanks

<?xml version="1.0" encoding="UTF-8"?>

Altair Forum User · January 2015

Hi Steveivy,

We are looking into the Nastran export issue you are facing.

Regarding the applied load, yes it is 10000N which is applied on the model. Have you used box selection to select nodes when applying force?

instead, select the two nodes which you are interested in by manually clicking on the nodes.

Altair Forum User · January 2015

Altair Forum User said:

Hi Steveivy,

We are looking into the Nastran export issue you are facing.

Regarding the applied load, yes it is 10000N which is applied on the model. Have you used box selection to select nodes when applying force?

instead, select the two nodes which you are interested in by manually clicking on the nodes.

I used 'select by window'. Or I can just divide the total magnitude by the number of layers and I will get the desired the total force.

Altair Forum User · January 2015

Yes,

you can do that. Instead of layers, prefer divide total magnitude with total number of nodes.

say if the total load is 1000N and you want to distribute on 10 nodes, then on each node the load is 1000/10= 100N

Altair Forum User · January 2015

Hi,

could you please let us know what is the version of HyperWorks installed on your machine and what are all the updates you have?

Please use the link below for information on how to check for updates:

http://forum.altairhyperworks.com/index.php?/topic/13435-to-identify-the-software-updatepatch-that-has-been-installed-in-your-machine/

Altair Forum User · January 2015

I think the problem is with the co-incident nodes.

If you count the number of nodes you will see that there are 8 nodes in the model.

Try equivalencing the nodes. Goto Tool page>> Edges>> select component>> Preview Equivalence to see free nodes.

<?xml version="1.0" encoding="UTF-8"?>

Altair Forum User · January 2015

Altair Forum User said:

Hi,

could you please let us know what is the version of HyperWorks installed on your machine and what are all the updates you have?

Please use the link below for information on how to check for updates:

http://forum.altairhyperworks.com/index.php?/topic/13435-to-identify-the-software-updatepatch-that-has-been-installed-in-your-machine/

Hi,

I am using 11.0 version. The code I posted originally was generated from 8.0. I will try your method when I get to school.

Altair Forum User · January 2015

Altair Forum User said:

I think the problem is with the co-incident nodes.

If you count the number of nodes you will see that there are 8 nodes in the model.

Try equivalencing the nodes. Goto Tool page>> Edges>> select component>> Preview Equivalence to see free nodes.

Hi,

I went to this point(see attached picture) and I don't know how to do next. I clicked preview equivalence but nothing going on. Thanks

<?xml version="1.0" encoding="UTF-8"?>

tinh · January 2015

Altair Forum User said:

Hi,

I went to this point(see attached picture) and I don't know how to do next. I clicked preview equivalence but nothing going on. Thanks

just due to you create node IDs 1, 2, 3, 4 then nodes 5,6,7,8 concide to 1,2,3,4

so press Shift+F2 => clear all => will clear all free nodes 1,2,3,4 (because your CBEAM refer to nodes 5,6,7,8 so SPC and FORCE should refer to them too)

Altair Forum User · January 2015

Altair Forum User said:

just due to you create node IDs 1, 2, 3, 4 then nodes 5,6,7,8 concide to 1,2,3,4

so press Shift+F2 => clear all => will clear all free nodes 1,2,3,4 (because your CBEAM refer to nodes 5,6,7,8 so SPC and FORCE should refer to them too)

Ok, I will try that. But I am just curious, I only create 4 nodes, how come there are 8 nodes IDs?

Thanks

Altair Forum User · January 2015

Hi Steveivy,

Please follow Tinh's suggestion.

if that doesn't work, you can use Tools page>> Edges>> slelect components/elements>> Equivalence.

if the problem still exists after doing this, you can replace nodes using Replace panel (F3 is the shortcut on your keyboard). Make sure you have activated coincidenct node picking in Options page (Press O on your keyboard>>Graphics>> coincident picking)

tinh · January 2015

Altair Forum User said:

Ok, I will try that. But I am just curious, I only create 4 nodes, how come there are 8 nodes IDs?

Thanks

perhaps you duplicated them, search if any '*duplicatemark nodes' command appeared in your \documents\command.cmf file

Altair Forum User · January 2015

Altair Forum User said:

Hi Steveivy,

Please follow Tinh's suggestion.

if that doesn't work, you can use Tools page>> Edges>> slelect components/elements>> Equivalence.

if the problem still exists after doing this, you can replace nodes using Replace panel (F3 is the shortcut on your keyboard). Make sure you have activated coincidenct node picking in Options page (Press O on your keyboard>>Graphics>> coincident picking)

Altair Forum User said:

perhaps you duplicated them, search if any '*duplicatemark nodes' command appeared in your \documents\command.cmf file

tinh

It works. Thank you guys

So in the future, will it be a good practice that clear all the free nodes before applying forces and constrains? And is there an easy way to tell that I have free nodes in the model?

tinh · January 2015

Yes Steveivy, free nodes appear in form of 'yellow balls' and you can easily see them

And you should activate 'concide picking' as Pagadala's suggestion to avoid wrong selection

Problem with exported Nastran code file

Answers

Categories