Modeling Joints as Surface Model

Technical Article

With RF-/FRAME-JOINT Pro, it is possible to design frame joints according to DIN 18800 or Eurocode 3. If it is about non-standardized joints or taking a closer look at the joint and its behavior, it is recommended to use the modeling as surface model. The following article will show how such a model is structured in principle.

Modeling the Member Model

RFEM offers the possibility to convert thin-walled cross-sections as members to surface models. Therefore, the member model should be created first and afterwards, the corresponding members should be converted. The model which is used in this article, is shown in Figure 01 a.

Figure 01 - Hall Frame as Basis for Surface Model

It is a single hall frame where the frame joint, highlighted with an arrow in the figure, will be replaced by a surface model. The length of the members plays an important role here from two points of view.

  1. A surface model requires many more FE elements than a member. Therefore, it is recommended to choose the length of the member as small as possible to minimize the calculation effort and thus the duration of the calculation. Otherwise, the calculation is more precise if even more FE elements and also a big part of the member is defined as surface model.
  2. The conversion from member to surface model requires a good load application since the member forces have to be transferred from a node to the lines of the cross-section. To receive a load distribution as realistic as possible, the member should not be too short.

In order to meet both requirements, the general rule of the load distribution at an angle of 60 ° can be used. The largest width of the cross-section should be applied at least as length for the area of the load application.

Figure 02 - Influence of Column Length

Figure 02 shows the comparison of three modeled frame joints in one section which has been applied at the half cross-section width w. The reference value is the von Mises equivalent stress. It is clearly evident that there are still bigger differences between option 1 with single and option 2 with double cross-section width with the length l. For more than the triple length in option 3, the differences can be hardly seen. Therefore, it is recommended to apply the double cross-section width as length to be on the safe side. The same applies to the girder. In the interests of simplification, a cut was not performed and the entire taper was used.

Since the column should be continuous, it has to be extended upwards by one more member. The member length should be selected in such a way that it protrudes at least over the taper, because it will be cut down to the right length later. The modified frame joint is shown in Figure 01 b.

Creation of the Surface Model

The members can now be converted to surface models. By right-clicking a member, the "Generate Surfaces" menu will open. The created model has, however, various intersections. Moreover, end plates, ribs and also a correct inclination of the column at the top are missing.

First of all, the intersections should be edited. The tool "Connect Lines/Members" can be used here. If two intersecting surfaces are selected, intersection points at the boundary lines at the interection are created. It would be also possible to create an intersection and to convert them to a line. The end points of the taper can be then moved to these new points as shown in Figure 03.

Figure 03 - Cutting the Taper with "Connect Lines/Members"

It is possible that surfaces become incorrect or are deleted. This can be corrected later. After having deleted all unnecessary lines and nodes, a model as shown in Figure 04 should be present.

Figure 04 - Transfer Girder Inclination to Column

The next step is the cutting to length of the column. To display the right inclination of the taper correctly, one of the edges of the upper flange is used for the displacement vector during copying. The process is displayed in Figure 04. The upper intersection point between column and girder flange is to be copied. In the "Move/Copy" dialog box, a copy is entered and selected as vector of the start and end node of the girder flange edge. Since the girder is reduced, the value for this direction (here dY) has to be set to 0. A line between both nodes can be created now. This line also intersects the opposite flange edge of the column now. With the tool "Connect Lines/Members", it is possible to generate the intersection point.

Figure 05 - Cutting the Column

After the correct inclination is displayed now, the new node is mirrored or copied to the other side of the column and the nodes of the column end are then moved to these new nodes (Figure 05 a). At this point, the joint between the column and the created extension can be moved to the lower edge of the taper and the additional lines for the stiffeners and the end plate can be created as shown in Figure 05 b.

Afterwards, the end plate of the taper will be created. The intersection lines between column and girder can be copied perpendicular to the column. The distance is dependent on the flange and end plate thickness. The half thickness has to be added in each case. In the present example, the flange has a thickness of 13.5 mm and the end plate a thickness of 12 mm. This results in a distance of about 13 mm. When the lines have been copied, the lines of the girder can be moved to the new nodes at the end as well (Figure 06) and the additional connection lines can be created for the end plate. After this step, the surfaces of the taper will be no longer present since the boundary lines have been changed.

Figure 06 - Create Node for End Plate at the Girder

To finish the modeling, rib lines and lost and new surfaces are created. This would result for the present case as shown in Figure 07. For a clearly-arranged display, the surfaces are shown in different colors depending on the thickness.

Figure 07 - Completed Surface Modeling with Additional Web Stiffeners

Modeling of Bolt/Flange Connection

The connection between end plate of the girder and flange of the column will be realized by using a contact solid and members. The contact solid is placed between the two surfaces (column/girder) and can simulate the failure under tension between the surfaces. The tension forces should be absorbed by the bolts which are modeled as members.

First of all, the drilled holes are created. The basis for the drilled holes are openings in flange and end plate. First of all, the node of the end plate at the top is copied to the right position (Figure 08 a).  At this location, a circle can be created (work plane has to be considered). Boundary surfaces of contact solids need to have always four boundary lines. Since this is not yet the case for this hole with its inner surfaces, the circle has to be separated in two segments (insert line and use "Connect Lines/Members"). With "Select Boundary Lines", the opening can be created (Figure 08 b).

Figure 08 - Create Hole Drillings at the Beam End Plate

In the next step, the generated drilled hole together with the center is copied to the bottom. Both drilled holes can then be mirrored (Figure 09 a). The contact solid or rather the two contact solids are created by clicking the opposite surfaces and selecting "Create Solid with Contact" (Figure 09 b). The completed contact solids are shown in the model in Figure 09 c. The characteristic "Failure under tension" is set in the dialog box of the solids.

Figure 09 - Completed Hole Drilling Opening and Creation of Contact Solid

Members with the cross-section round steel can be used for modeling the bolts with regard to the core diameter of the used bolts. A prestress can be applied. The connection between member and surface is carried out with a surface of the type "Membrane - Without Tension". The failure under tension is thus simulated in the hole bearing (Figure 10).

Figure 10 - Completed Modeling of the Frame Joint with Bolts and Rigid Members

The connection to the member model is created by rigid members. Rigid members are created at both ends of the cross-section outlines of the surface model which ensure a uniformly distributed load application of the point from the member to the surface model.

Handy Hints

If the modeling is coherent will be obvious when generating the FE mesh. In the following, three typical issues and how to solve them will be presented.

  1. "The definition lines of a surface are not closed"
    This issue occurs if boundary lines of a surface have been modified. In this case, several surfaces of the taper were concerned. These old surfaces have been already replaced by new surfaces and the old incomplete surfaces can be deleted. Generally, it can be stated that correcting a surface takes often longer than generating a new one with "Selecting Boundary Lines".
  2. "Numbers of integrated objects in contact surfaces do not correspond"
    When using a contact solid, both contact surfaces have to be absolutely identical. Where a node is present in a surface, the node has to be also present along the surface normal in the other surface. The boundary surfaces have to be ordinary to both contact surfaces everywhere as well.
  3. "Side surfaces XX do not have four boundary lines"
    All side surfaces of a contact solid need to have four boundary lines. This also applies to holes in a contact solid. Figure 11 shows a little example. In case a, the displayed boundary surface has exactly four lines (2, 22, 10, 23), in case b, however, five which is not allowed. The number of boundary lines of the contact surfaces is, however, not relevant.
Figure 11 - Correct and Wrong Modeling of Boundary Surface of a Contact Solid

Keywords

modeling connection surface model

Downloads

Links

Contact us

Contact Dlubal Software

Do you have any questions or need advice?
Contact us or find various suggested solutions and useful tips on our FAQ page.

(267) 702-2815

info-us@dlubal.com

RFEM Main Program
RFEM 5.xx

Main Program

Structural engineering software for finite element analysis (FEA) of planar and spatial structural systems consisting of plates, walls, shells, members (beams), solids and contact elements

Price of First License
3,540.00 USD
RFEM Connections
RF-FRAME-JOINT Pro 5.xx

Add-on Module

Design of rigid bolted frame joints according to Eurocode 3 or DIN 18800

Price of First License
1,120.00 USD
RFEM Connections
RF-JOINTS Timber - Timber to Timber 5.xx

Add-on Module

Design of Direct Timber Connections According to Eurocode 5

Price of First License
360.00 USD
RFEM Connections
RF-JOINTS Timber - Steel to Timber 5.xx

Add-on Module

Design of indirect timber connections with dowel-type fasteners and steel plates according to NDS and Eurocode 5

Price of First License
850.00 USD
RFEM Connections
RF-JOINTS Steel - DSTV 5.xx

Add-on Module

Design of standardised joints in steel structures according to the EN 1993‑1‑8 - DSTV guideline

Price of First License
670.00 USD
RFEM Connections
RF-JOINTS Steel - Pinned 5.xx

Add-on Module

Design of pinned joints according to Eurocode 3

Price of First License
670.00 USD
RFEM Connections
RF-JOINTS Steel - Tower 5.xx

Add-on Module

Design of nominally pinned bolted connections of members used in lattice towers according to Eurocode 3

Price of First License
670.00 USD
RFEM Connections
RF-JOINTS Steel - SIKLA 5.xx

Add-on Module

Design of SIKLA joints according to GX K14-6005-3

Price of First License
1,120.00 USD
RFEM Connections
RF-JOINTS Steel - Column Base 5.xx

Add-on Module

Design of hinged and restrained column base footings according to Eurocode 3

Price of First License
670.00 USD