Hole to hole fastener mesh 5

[joneseyeng]

I am brand new to FEMAP and FEA type software. I am trying to use the hole to hole fastener mesh under custom tools to create a mesh for my fastener holes. I have a lot of fasteners in my model and everytime I create a mesh it creates a new property. I really do not want to keep track of 100+ properties for my fasteners. Is there an easier way to do this or can I combine my properties somehow? Thanks for any assistance I am very new to this program.

 

[rb1957]

you can use the modify command to update element property, you might be able to simply select all elements and update to a single property, certainly (i think) you can select elements by property, select properties 2 thru n, that'll select all the elements you want to change, change to property 1 ...

 

[DMoreno]

Hey joneseyeng, if you don't want to end with the multiple fastener properties created by the hole2hole macro, before using it You must first select and make active the property that You created manually with the beam property for the fastener or stop the macro right after the first fastener and select and make active the property recently created. Then you can continue with the macro and all the following fasteners will have the property assigned.

Best regards
Diego Moreno

 

[AndyFEMAP]

joneseyeng,

DMoreno's comments are correct and may be helpful. In addition, I would like to offer you an API that I created to automatically make bolt elements by selecting all the curves in an area of the model. It looks for "loops" which make up holes, so if you pick some extra curves, it shouldn't matter. This version actually asks if you want to use an existing Beam property, CBUSH property (If so, creates coincident node CBUSH elements), or enter a bolt radius. If you enter a bolt radius, all elements created will use the same Property.

Please post any questions, comments or concerns about this API on this thread and I will do my best to answer them. In addition, if you already have "hundreds" of API fastener properties, I could also write a "property consolidation" API for the fastener elements which may be helpful. Please let me know.

Thanks,

Andy - FEMAP development

Code starts here:

Sub Main
Dim App As femap.model
Set App = feFemap()

Dim Cu As femap.Curve
Set Cu = App.feCurve

Dim cuSet As femap.Set
Set cuSet = App.feSet

Dim CircSet As femap.Set
Set CircSet = App.feSet

Dim CircSubSet As femap.Set
Set CircSubSet = App.feSet

Dim FinSet As femap.Set
Set FinSet = App.feSet

Dim PointSet As femap.Set
Set PointSet = App.feSet

Dim IndNdSet As femap.Set
Set IndNdSet = App.feSet

Dim feNode As femap.Node
Set feNode = App.feNode

Dim nodeSet As femap.Set
Set nodeSet = App.feSet

Dim feElem As femap.Elem
Set feElem = App.feElem

Dim DeleteSet As femap.Set
Set DeleteSet = App.feSet

Dim El As femap.Elem
Set El = App.feElem

Dim P As femap.Prop
Set P = App.feProp

Dim pset As femap.Set
Set pset = App.feSet

Dim listtype(0) As Long
Dim entityID(0) As Long
Dim FaceID(0) As Long
Dim Expanded(0) As Long

Dim BoReg(0) As Long
Dim BoVal(0) As Double

Dim Preload As Double

Dim BeamElID As Long
Dim PropID As Long
Dim BeamID As Long
Dim RAD As Double

Dim cuCenter As Variant
Dim cuNormal As Variant
Dim cuStartPt As Variant
Dim cuEndPt As Variant
Dim cuAngle As Double
Dim cuRadius As Double

Dim nd1loc(2) As Double
Dim nd2loc(2) As Double
Dim dist As Double
Dim DistCurrent As Double

Dim pt1 As Long
Dim pt2 As Long

Dim nodeCount As Long
Dim nodeX As Double
Dim nodeY As Double
Dim nodeZ As Double
Dim nodeID As Long
Dim elemID As Long
Dim vNodeArray As Variant

Dim BeamArea As Double
Dim Vec(3) As Variant
Dim X As Double
Dim Y As Double
Dim Z As Double
Dim X1 As Double
Dim Y1 As Double
Dim Z1 As Double
Dim VecP As Variant

Dim feMatl As femap.Matl
Set feMatl = App.feMatl
Dim matID As Long

rc = App.feAppMessageBox (3, "Select Existing Beam or Spring-CBUSH Property (No=Enter Bolt Radius)")

If rc=2 Then
GoTo Done
End If

If rc=0 Then

matID = App.Info_ActiveID( FT_MATL )

If matID = 0 Then
Msg = "No active material for fastener, please activate a material and re-run."
rc = MsgBox( Msg, vbOkOnly, "No Material" )
GoTo Done
End If

rc = feMatl.Get( matID )

'Section Values A

Radagain:

rc = App.feGetReal ("Enter Bolt Radius", 0.000000001, 1000000, RAD)
If rc = 2 Then
GoTo Done
End If

PropID = P.NextEmptyID
P.title = "API Fastener"
P.type = FET_L_BEAM
P.flagI(1) = 5
P.pval (40) = RAD
P.ComputeShape (False, False, True)
P.matlID = matID
P.Put(PropID)
Proptype = P.type

Else
again:
rc = pset.SelectID (FT_PROP, "Select Beam Property for Bolt", PropID)
If rc = 2 Then
GoTo Done
End If
P.Get (PropID)
proptype = P.type
If proptype <> 5 Then
If proptype = 6 Then
isBush = P.flag(3)
If isBush = True Then
refCSYS = P.flag(0)
If refCSYS = True Then
GoTo MoveOn
Else
rc = App.feAppMessageBox (1, "Selected Spring Property does not have Orientation CSys defined. Select Different Property?")
If rc = 2 Then
GoTo Done
Else
GoTo Again
End If
End If
Else
rc = App.feAppMessageBox (1, "Selected Spring Property is not set to CBUSH. Select Different Property?")
If rc = 2 Then
GoTo Done
Else
GoTo Again
End If
End If
Else
rc = App.feAppMessageBox (1, "Selected Property is not a Beam or Spring Property. Select Different Property?")
If rc = 2 Then
GoTo Done
Else
GoTo Again
End If
End If
End If
End If

MoveOn:

cuSet.Select (FT_CURVE, True, "Select Curves for Bolts")

cuID = cuSet.First

While cuID > 0
Cu.Get(cuID)
rc = Cu.ArcCircleInfo( cuCenter, cuNormal, cuStartPt, cuEndPt, cuAngle, cuRadius )
If rc = FE_OK Then
CircSet.Add (cuID)
End If
cuID = cuSet.Next
Wend

CircID = CircSet.First

While CircID > 0
Cu.Get(CircID)
Cu.EndPoints (pt1, pt2)
CircSubSet.AddRule (pt1, FGD_CURVE_BYPOINT)
CircSubSet.AddRule (pt2, FGD_CURVE_BYPOINT)
CircSubID = CircSubSet.First
While CircSubID > 0
Cu.Get(CircSubID)
Cu.EndPoints (pt1, pt2)
CircSubSet.AddRule (pt1, FGD_CURVE_BYPOINT)
CircSubSet.AddRule (pt2, FGD_CURVE_BYPOINT)
CircSubID = CircSubSet.Next
Wend
FinSet.AddCommon (CircSet.ID, CircSubSet.ID)
CuNum = FinSet.Count
PointSet.AddSetRule (FinSet.ID, FGD_POINT_ONCURVE)
PtNum = PointSet.Count
If CuNum <> PtNum Then
GoTo Skip
End If

' Get a set of nodes for this rigid element

rc = nodeSet.AddSetRule( FinSet.ID, FGD_NODE_ATCURVE )

If nodeSet.Count = 0 Then
App.feAppMessageBox (0, "No nodes exist on a selected curve(s). Exiting...")
GoTo Jumping_Out
End If

'Lets see how many nodes were selected
nodeCount = nodeSet.Count()

If nodeCount > 0 Then
' Walk the nodes and find the average
rc = nodeSet.Reset()
nodeID = nodeSet.Next()
ReDim nodeArray(nodeCount) As Long

Dim passCount As Long

passCount = 0

Do While nodeID <> 0

nodeArray(passCount) = nodeID
passCount = passCount + 1
rc = feNode.Get(nodeID)

nodeX = nodeX + feNode.x
nodeY = nodeY + feNode.y
nodeZ = nodeZ + feNode.z

nodeID = nodeSet.Next()

Loop

vNodeArray = nodeArray

nodeID = feNode.NextEmptyID

feNode.ID = nodeID
feNode.x = nodeX / nodeCount
feNode.y = nodeY / nodeCount
feNode.z = nodeZ / nodeCount

rc = feNode.Put(nodeID)
IndNdSet.Add (nodeID)

If rc = -1 Then 'return code FE_OK
' create the element

elemID = feElem.NextEmptyID
feElem.type = FET_L_RIGID
feElem.topology = FTO_RIGIDLIST

feElem.Node(0) = nodeID 'Independent Node
feElem.release(0, 0) = 1
feElem.release(0, 1) = 1
feElem.release(0, 2) = 1

feElem.ID = elemID

rc = feElem.PutNodeList(0, nodeCount, vNodeArray, Null, Null, Null)
rc = feElem.Put(elemID)

nodeCount = 0

rc = nodeSet.Clear()

nodeX = 0#
nodeY = 0#
nodeZ = 0#
End If
End If
Skip:
PointSet.Clear
CircSet.RemoveSet (FinSet.ID)
FinSet.Clear
CircSubSet.Clear
CircID = CircSet.Next
Wend

If IndNdSet.Count = 1 Then
Nd1 = IndNdSet.First
DeleteSet.AddRule (nd1, FGD_ELEM_BYNODE)
feElem.Delete (DeleteSet.First)
feNode.Delete (Nd1)
GoTo Jumping_Out
End If

nd1 = IndNdSet.First
While nd1 > 0
feNode.Get(nd1)
nd1loc(0) = feNode.x
nd1loc(1) = feNode.y
nd1loc(2) = feNode.z
DistCurrent = 1000000.0
nd2 = IndNdSet.Next
IndNdSet.Remove (nd1)
While nd2 > 0
feNode.Get(nd2)
nd2loc(0) = feNode.x
nd2loc(1) = feNode.y
nd2loc(2) = feNode.z
App.feMeasureDistance (nd1loc, nd2loc, dist)
If DistCurrent > dist Then
DistCurrent = dist
nd2Keep = nd2
End If
nd2 = IndNdSet.Next
Wend
IndNdSet.Remove (nd2keep)
IndNdSet.Reset

BeamElID = El.NextEmptyID
If Proptype = 5 Then
El.type = FET_L_BEAM
Else
El.type = FET_L_SPRING
End If
El.Node (0) = nd1
El.Node (1) = nd2Keep
rc = feNode.Get (nd1)
X = feNode.x
Y = feNode.y
Z = feNode.z
rc = feNode.Get (nd2Keep)
X1 = feNode.x
Y1 = feNode.y
Z1 = feNode.z
Vec(0) = X - X1
Vec(1) = Y - Y1
Vec(2) = Z - Z1
rc = App.feVectorPerpendicular (Vec, VecP)
El.orient(0) = VecP(0)
El.orient(1) = VecP(1)
El.orient(2) = VecP(2)
El.propID = PropID
El.Put (BeamElID)

If proptype = 6 Then
newx = (X + X1) / 2
newy = (Y + Y1) / 2
newz = (Z + Z1) / 2

feNode.x = newx
feNode.y = newy
feNode.z = newz

rc = feNode.Put(nd1)
rc = feNode.Put(nd2Keep)
End If

If IndNdSet.Count = 1 Then
Nd1 = IndNdSet.First
DeleteSet.AddRule (nd1, FGD_ELEM_BYNODE)
feElem.Delete (DeleteSet.First)
feNode.Delete (Nd1)
GoTo Jumping_Out
End If

nd1 = IndNdSet.First
Wend

Jumping_Out:

Call App.feViewRegenerate(0)

Done:

End Sub

 

[DMoreno]

Hi AndyFEMAP, would be Ok with You if I use the program to try it out FEMAP v10.3.1?
Best regards

 

[AndyFEMAP]

By all means, please give it a try. I posted it for everyone to use. Also, when choosing a property, the type of property selected is used to determine the type of elements to create. When selecting a Spring/Damper property, it "should" provide a warning unless you select a "Spring/Damper" property set to CBUSH which also has "Orintetation CSys" turned on.

 

[BlasMolero]

Dear Andy,
A star for you!!. Very good API, after testing a few suggestions:

• After creation of the spider + bolt to continue asking for curves for bolt creation, now the API ends after the bolt creation, and again is required to answer if select existing beam properties or create a new one. Only ask for it the first time, if required a new property then the user will stop simply hitting ESC command.
• CBeam Stress recovery points are missing in the beam properties definition for bolt elements.

Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/