1 / 20

TUTORIAL 3 LOADING, CONSTRAINTS, AND MODEL CLEANUP

TUTORIAL 3 LOADING, CONSTRAINTS, AND MODEL CLEANUP. Note: As in the other tutorials, all menu items that need to be selected will be preceded

ayala
Download Presentation

TUTORIAL 3 LOADING, CONSTRAINTS, AND MODEL CLEANUP

An Image/Link below is provided (as is) to download presentation Download Policy: Content on the Website is provided to you AS IS for your information and personal use and may not be sold / licensed / shared on other websites without getting consent from its author. Content is provided to you AS IS for your information and personal use only. Download presentation by click this link. While downloading, if for some reason you are not able to download a presentation, the publisher may have deleted the file from their server. During download, if you can't get a presentation, the file might be deleted by the publisher.

E N D

Presentation Transcript

  1. TUTORIAL 3LOADING, CONSTRAINTS, AND MODEL CLEANUP

  2. Note: As in the other tutorials, all menu items that need to be selected will be preceded by a maroon right arrow: >User action. Mouse buttons are indicated as follows: -- 1B = First (left) button -- used for selecting items-- 2B = Second (middle) button -- used for "OK"-- 3B = Third (right) button -- used for View Manipulation & pop-up menusNormally 1B is used, unless otherwise. Table Of Contents • SectionPage • Step1. Open MSC.SOFY Database. 3 • Step2. Create Hole. 4 • Step3. Create RBE2 rigid spiders. 5 • Step4. Create SPC’s. 6 • Step5. Apply Force. 7 • Step6 . Create Pressure Loading. 9 • Step7 . Create Enforced Displacement. 12 • Step8 . Some model checks and cleanup 13 • Step9 . Diagnose and fix weld normality and other rigid element errors. 14 • Step10. Model Cleanup. 15 • Step11. Export Nastran Deck for static analysis . 17 • Step12. Create additional cards. 18

  3. Step1. Open MSC.SOFY Database. e • Launch MSC.SOFY according to your local configuration. • Choose >Nastran from the entry screen. • From >File menu, >Units Mgr> select >Standard Units: >NASTRAN without WTMASS card. • Open the SOFY database of a Decklid model like the one we used in Tutorial N-2: • File >Open. • In the File Open dialog, browse to the file: N-3_decklid_start.sof and >Open.

  4. Step2. Create Hole. a • We'll be putting some constraints at the hinges. But first we • need to properly mesh and attach the bolt holes. • Zoom into the left hinge area. • Turn >Off the >Decklid Outer. • There are holes in the inner panel, but not on the reinforcement. • From >Mesh menu> select >Create Hole with Washer to create on the reinforcement. • You are prompted to select parts, so pick just the >Reinf_Hinge from the canvas. • Confirm with >2B. • Now to pick the hole center: Select > node to define hole center which lines up with existing hole on the inner panel. • Confirm with >2B. • (If node is not present at desired center point, use >Pt on Element pick type.) • Enter the parameters as shown in the dialog box. • Click >OK to create the hole. • Repeat for other hole location and >Exit. i

  5. Step3. Create RBE2 rigid spiders. c • Now put a rigid "spider" at each of the hole locations: • Create a new part called >Bolts. • Select >Element >Create >Rigid >RBE2. • In the Pick block> select >Ind Node at Mid Loc. • Select >Nodes as the pick entity type (default) • Use >Sketch pick style to select all the nodes around the hole for the two parts. • Confirm with >2B and the rigid spider is created. • Repeat for the other hole. • Go to other side of model and >Create Hole with washer & RBE2 rigid spiders at both bolt holes. f

  6. Step4. Create SPC’s. d e • Now to create some SPC's.... • Collection Block>click >All On to bring back all parts to the display. • Change >Type to >BC Set. (Boundary Condition Set) • Right click (>3B) in list area • Click >Create from pop-up menu. • In dialog box, type in the name >hinge_spc for the new BC Set >Create and >Exit the dialog. • Select >BC >Create BC >SPC. • In the pop-up make sure the boxes are checked for all six DOF's. • Click >Store • Click >Exit. • Now select the center >node of each rigid spider created above (two on each side). • Confirm with >2B to create the SPC's. • Click >Exit Pick block. g k

  7. Step5. Apply Force. • Let's apply some forces: • Create another BC Set called >torsion. • Zoom into the lower rear corner of the decklid. • Select >BC >Create BC >Force. • In the pop-up, enter F= 50, DIR1= 0, DIR2= 0, and DIR3= 1. • Click >Store and >Exit. • In Pick block>Coordinates >Global . • Thus each force will be 50N in Z direction. • Pick two nodes near the corner of the decklid inner. • Click >Done. • If you wish to pick only the independent nodes of rigid elements, you can identify them using • 1. Utilities >Identify. • 2. Set >Details On from toolbar. • 3. Pick block> select >Elements • 4. Pick the rigid >element of interest. • 5. Each end will then be labeled as "I" or "D" • as appropriate. d f c a i

  8. Step5. Apply Force. (Cont’d) • Repeat loading on opposite side, except make load in opposite direction. • In Pick Block>Click >(Defaults) button • Change >DIR3 to -1 in dialog box. • Click >Store. • Pick two corner >nodes as was done in Step 5-h. • Click >D (Done). m

  9. Step6. Create Pressure Loading. • We'll be applying a pressure load over an area on the top surface of the decklid. • Create a new BC Set named >Surface. • Use >Organize command to >Keep only the Decklid outer parts (2). • Use >Distance icon to identify an area in the center of the decklid sized at 200mm X 200 mm. • Create a temporary new part called >Temp. • Element menu> select >Move to Curr Part. • Use >Polygon pick style> Select >elements within the 200 X 200 area. • Confirm with >2B • Elements are moved to the new part. • Turn >off all parts except for >Temp. • Click drop >arrow next to Mass icon (on Query Utils toolbar). • Select >Area from drop-down menu, • Check that the area of the new parts is at about 40,000 mm2. • If not, move elements to/from the part "Temp." • From >BC menu> select >Create BC >PLOAD2. • In the dialog> enter pressure of > 0.02 N/mm2. • Select >All elements in the part >Temp • Confirm with >2B. g

  10. Step6. Create Pressure Loading. (Cont’d) • There are problems with the element normals in this model. • Let's fix the normals. • Click >Details On icon • You can see that one half of the part has the pressure loading in the wrong direction. • We must fix the element normals. • Turn BC Sets >All Off in Collection block. • From >Element menu> select >Normals. • In Pick block>Choose >Show Normals from drop-down box. • Select >Disp (Displayed) elements. • Click >Done. • After checking the normals you can change the drop-down to >Fix Normals. • You are prompted to pick a Reference >element. • Choose an element with the correct normal direction as the seed element. • Refresh the display to check that normals are corrected. • (You can also use >Reverse normals option to reverse selected elements.) • The Decklid Outer needs to be corrected also • Before leaving the Normals command, • Select>Hide Normals (from drop arrow)> select >All elements • Click >Done to remove normals from the display. • Now >Exit. f

  11. Step6. Create Pressure Loading. (Cont’d) • Delete and re-create the incorrect pressure loads created above: • Collection block >Type >BC Set> turn on >Surface. • From BC menu >Delete. • Using Polygon or Window pick style> select >all pressure loads. • Confirm with >2B, • Now >Exit the command. • Select >BC >Create BC >PLOAD2 • Follow the same procedure as in step 9, above. • This time the pressure load should be all in the same direction. • Turn on only the parts: • >Decklid outer • >Decklid outer.Copy • >Temp. • Make >Decklid Outer the Current part >click with >2B. • From >Element menu> select >Move to Curr Part. • In Pick block click >All. • Click >Done.

  12. Step7. Create Enforced Displacement. a • Create a new BC Set >Lateral. • Create enforced displacement using >BC >Create BC >SPC. • Uncheck all DOF's except for >D2. • Put a value of 5.0 in the field for >D2. • Now pick a >node or two on the side of the decklid, near the bottom, • Confirm with >2B. b

  13. Step8. Some model checks and cleanup • Let’s check the overall quality of this model. • From >Element menu> select >Quality >Check Quality. • In the Quality Check form > click >Restore Defaults near bottom of window. • Make sure the boxes are checked for >Quality Checks and >Element Checks. • Also, check the box for >Output file. • Click >OK at bottom. • The file "quality.out" should pop up in a text editor window. • Browse the file to see the quality diagnostics. • Note there are several serious errors in this model. • The most serious are precede with 4 stars (****) relate to Rigid loops and Bad Dependency problems. esp weld normality. • Let's try to fix those first. • The failed elements are highlighted in the canvas and are also placed into Sets in MSC.SOFY. • In Collection block > change >Type >Set. • Click >3B over the set >Bad Dependency. • In the pop-up> select >Equal. • This has the effect of displaying only elements in the set, so you can easily find the failed elements. • To fix these elements, • Element >Quality >Remove Dbl. Dep. • Watch message area, and it will indicate if the elements were fixed. (e.g. "4 Rigids Switched ") • Back in Collection block >click >3B over the Set >Duplicate elements . • There are two locations along the centerline of the decklid where duplicate Rigids exist. • Delete one or more rigid element in each location to eliminate the problem. (Element >Delete) • When finished, there may also be coincident nodes at those locations. • Use >Node, >Merge Coin. Node command to resolve.

  14. Step9. Diagnose and fix weld normality and other rigid element errors. • There are many elements which failed the Weld Normality check, mostly along the rear edge. Let's see if we can fix • them.... • Click >3B over the Set >Weld Normality • Click >Equal in pop-up. • Select >Grow Mesh icon a couple of times to bring up surrounding elements. • Turn >Fringes On to see color fringes of quality. • Let's try and fix with automatic quality enhancement: • Element >Quality >Enhance Quality. • Select >All when prompted to pick elements • Click >Done. • In the Quality Enhance pop-up, • enter >100> "Num of Weld Normality Enhancing passes" • enter > 0.5> "Tolerance". • Click >Enhance. • The file "compare.out" pops up in a text editor window showing the statistics on how successful the quality enhancement was. • In this case, we may not be able to fix all the weld normality because the two connected panels are angled from one another and the failed elements are along a boundary. • You can repeat the >Enhance Quality process again to further improve Or consider increasing the max allowable value in the Quality Check form. • Turn parts >All On and >Unmask everything. • Check Quality again, and use >Enhance Quality command again, as needed, to further improve element quality.

  15. Step10. Model Cleanup. c • Let's move on. We'll perform some model cleanup, such as duplicate ID's, unreferenced materials, etc • From >Utilities menu> select >ID Mgmt >Diagnose Model ID's. • A window will pop up with the results, showing one duplicate part (PID #1). • To renumber the parts: • Utilities >ID Mgmt >Model ID Manager. • In the dialog box, you can activate the renumbering of any entity type by checking the boxes to the right. • Let's activate: >Parts, Nodes, Elements, and BC Sets. • Type in the start ID's and Offsets as shown. • Click >OK • For control over numbering of individual elements, nodes, etc., • Select >Utilities >ID Mgmt >Entity ID Manager. • In this case we can demonstrate by renumbering only the four grids at the hinges where we placed SPC's. • In Pick block> select entity type of >Nodes (default). • Now >Zoom in >select the >nodes at the rigid spider center on the part "bolts.“ • Confirm, then in the "Node ID Manager" pop-up, enter >1 as the starting ID for the four nodes. • Click >OK

  16. Step10. Model Cleanup. (Cont’d) • To lock the node numbers so they cannot be renumbered, • Utilities >ID Mgmt >Lock Entity ID's. • The box labeled "Unlock ID's" should be un-checked. • Now pick the same four nodes you just renumbered >Done. • They are now locked until you unlock them in the same fashion. • You may have noticed in the Quality checks that some materials and parts are empty or unreferenced. • To eliminate them, • Utilities menu>select >Model Cleanup>Select >Delete Unref'd. • In the Dialog box> click >Reverse to flip all selections from un-checked to checked. • Then hit >Apply. • Watch message area for indications of empty Parts, unreferenced Materials, unreferenced Nodes, etc. which are automatically deleted. • On Query Utilities toolbar >click >Mass icon. • The reported mass is unrealistically high. Let's investigate. • Clone the Collection Block and enlarge. • Click on >Info button > select >Thickness, >Mass, >Mat Shell, >Mat Solid, ># of Elements, and ># of Nodes. • We can see that the "Gumdrop" parts are responsible for the large mass. • Correct the material density for the gumdrop. • Change >Type in Collection Block to >Material. • Click >3B over material ID 2 (NEWMAT) • Click >Modify. • Change the density to a more realistic value, say 2.0E-6. • Change the name to >Gumdrop. • Click >Modify, and >Exit.

  17. Step11. Export Nastran Deck for static analysis . • We're just about ready to export the Nastran deck. • Add or Modify PARAM cards by changing >Type in Collection block to >Control. • Modify any of the cards listed by clicking with >3B and >Modify. • Finally ready to export the Nastran deck. • Set >Options >I/O Opts >Nastran Opts >Output opts. • Check the all the boxes, except those relating to Precision -- leave those at >Single precision. • Click >Exit (to exit the Options panel.) • Now to export the deck: • 1. File >Export >Nastran Model. • 2. Give the file an appropriate name, such as >decklid_static.nas. • 3. Click >Save. • At this point you can do the final editing of Exec Control and Case Control in any text editor.

  18. Step12. Create additional cards. • If a normal modes analysis is desired, you can createEIGR or EIGRL cards from Collection block: • 1. Change >Type to >Eigen Freq. • 2. Click >Create > choose >EIGR or >EIGRL card for normal modes analysis. • You can also createFREQ, FREQ1, or FREQ2 cards for Frequency Response analysis. • Similarly, from Collection Type >Global BC, you can create cards such as: RLOAD1, RLOAD2, TLOAD1, TLOAD2, LSEQ, and GRAV. • In Collection Type >Nastran Set, the following cards are available: DLOAD, ELIST, LOAD, MPCADD, SEELT, SESET,SET1, SPCADD, and USET1. • Finally, in the Collection Type >Tables, you can create various table cards, such as TABLED1,TABLED2,TABLEM1,DTABLE, etc. • Generally the card images available in Collection block are those that apply to the entire model or are not tied to a specific grid or element. • Loading cards that apply to specific elements or grids are located on the >BC >Create BC menu. (For example :FORCE,MOMENT, TEMP, SUPORT, DAREA.) • Exit MSC.SOFY: >File, >Quit. (Don't save.) • Congratulations!!! • You have just completed Nastran Tutorial 3.

More Related