Simulation: Weldments-Structural Member vs Weld Bead

SOLIDWORKS How To Questions
1

I’ve been modeling a recumbent bicycle frame based on a sketched centerline wire frame and using the Weldments - Structural Member feature with custom round tube profile sketches for modeling(extruding) 3D tubes along the centerline wire frame. Currently the model is a single SW part (not an assembly).
Recumbent Bike Frame Model.jpg
Shown below are the rear dropouts and their joints to the chainstays and seatstays. I’ve highlighted(blue) the (temporary version of the) right chainstay’s “pinched” joint model part into which one of the right dropout’s tabs is inserted.
Dropouts & Stays Screen Shot.jpg
I will eventually use Simulation for stress/strain analysis. The real frame is TIG welded and I’d like to have Simulation take the TIG welded joints into account in analysis if possible.

[ Questions ]

1. How does SW Simulation interpret a tube to tube joint modeled via the Weldments → Structural Member feature? Is the joint considered as if it were one piece - as if it were milled from one solid block of steel? Or would the joint be considered like a welded joint?

2. There is a separate Weld Bead feature. How is application of this Weld Bead feature along the joint of 2 individual tube parts different from the Structural Member modeled joint(in a single SW part)?

3. If I want to simulate the actual frame’s TIG welded tube joints, is there a way to continue using the Weldments → Sturctural Member feature generated frame model while taking advantage of the Weld Bead feature’s assignable settings?

4. The rear dropouts and the mock chainstay/seatstay “pinched” joints were obviously not modeled with Weldments features at all. But as the overall model is a single SW part, how would Simulation consider the “pinched” joint(w/o any weldment features intentionally applied) between the rear dropouts and the chainstays/seatstays? Would the “pinched” joint parts (like the highlighted one) be considered as a “unified” part with the chainstay and the dropout or would the “pinched” parts and the dropouts all be considered separated from the chainstays & seatstays?

Thanks~

2

Perhaps a summarized single question might invite someone to take a bite at this…

What’s the difference between a Weldments - Structural Member feature generated joint and a Weldments - Weld Bead feature generated joint once the model is opened within Simulation’s analysis environment? (i.e. How are the joints “perceived” differently by the “mind” of SW Simulation?)

Thanks~

3

Apparently, SW Simulation categorizes solid models based on 3 main meshing options*;
*Listed from the most simple to most complex - hence quickest to slowest to process

Mesh Types Based on Geometric Features

  1. Beam Mesh
  2. Shell Mesh
  3. Solid Mesh

Regarding the Weld Bead feature, I’ve encountered some comments online suggesting that it is purely a visual feature intended for accentuating weldments for example in drawings, and are supposedly not considered in say a static analysis in Simulation. Please correct me if this is not true (confirmations are also welcome).

When a frame/chassis or its member is modeled with the Weldments - Structural Member feature, apparently by default it is treated as “beam elements which have joints at junctions and connection points”.

Depending on priorities and/or preferences, the meshing method can be changed from say the default Beam to Shell or Solid Mesh, and the criteria to consider is described in the following site;

Regarding ‘Setting up a Static Simulation on SOLIDWORKS Weldments’, if the error
“Load/Restraint cannot be applied to the beam face, edge, or vertex”
is encountered the solution is to change the mesh from a default Beam Mesh to a Solid Mesh.

If anyone would like to add their experiences regarding this topic, I’m all ears!

Cheers~

4

I never used “Structural Member” or “Beam” in sim, on both IV and SW.
I always mesh them. It work only when everything is simple beams.

By default all contacts are “bonded” ie solid as one body.
Technically a proper weld is consider to be “same or better strength as rare material”.
Unless weld is not continuous.

You can set touching parts contact to “separate” or “sliding”. Model weld prep and weld. “Bond” weld to both part.
You may want to test a single weld before run the sim on whole model.
Analysis weld at the end after your frame is finish.
No point testing weld if the frame is not strong enough.

And I’m only talking about static sim.

5

Thanks Frederick, sorry for the delayed reply… I wanted to first wrap up my initial ‘exposure’ to linear(matrix) algebra, solid/continuum mechanics, and FEA basics* as well as Simulation so I could contribute some useful information.

  • Thanks to U.of Alberta Prof. Clayton Pettit’s online lectures(downloadable with apps) on YouTube!!! His lecture/seminar videos are better than the “OOO for Dummies” series. For those grossed out by 6X6+ matrices, integrals, partial derivatives etc. his lectures are the bomb - demystifies all the fancy geek gibberish.

As you mentioned, SW Simulation treats joints by default as ‘Bonded’ but apparently can be user defined - i.e. changeable to ‘Contact’(No Penetration), or ‘Free’(Allow Penetration).

Aside from the Weld Bead feature in SW (not applicable in Simulation), in SW Simulation, there is the ‘Edge Weld Connector’ (under ‘Connections’ along with Spring, Pin, Bolt, Bearing, … etc.)

*Note: ‘Connectors’ are “virtual” meaning ‘no (real) geometry’, hence no stress calculations or data result, but data regarding loads/forces transferred through them ARE analyzed) which allows analysis & determination of weld bead size based on user defined parameters such as electrode(welding rod) type, applied loads, estimated bead size, Factor of Safety etc.
It is amazing that “Weld Check Plot” in Simulation will show if a weld bead “Needs attention”(in size) or if it is “OK” based on comparison between the user’s “Estimated” bead size vs the analysis determined ‘required minimal bead size’ !

Further, within Weld Check Plot > “Details”, forces acting on the joint (i.e. Joint Normal Force, Shear-Weld axis force, Shear-Surface normal force, Bending moment, etc. ) can be viewed, and “Report Options” > “Plot” will display a graph of the required “Weld size”(leg length) and “Weld throat size”(depth from root to face).

As a SW rep mentioned in a seminar, it may be better though to initially do simulations without the Edge Weld Connector, and just utilize the default ‘Bonded’ feature for initial analysis data as the joint edge data will not be affected by idealized weld beads between the parent materials.
I think I will do both - first without Edge Weld Connector, then with the Edge Weld Connector activated for all joints, for comparative analysis.

For Simulation analysis with weld beads as the ONLY joining method (i.e. ‘Bonded’ Connection feature disabled), the following setup is possible;

  • Under Connections > Component Interactions > Global Interaction(Contact) > Edit Definitions,
    1.) Change the Interaction Type from ‘Bonded’ to ‘Contact’(No Penetration)
    2.) Set Properties > Gap range to consider contact > set gap dimension for inclusion of surfaces with gaps.

*** Important Note:** Tube/Pipe members generated with Weldments - Structural Member feature are recognized in Simulation (initially by default) as ‘Beams’ and their outer faces are NOT ‘select-ready’ as is (for application of the Edge Weld Connector features → a pop-up message will alert that the Edge Weld Connector feature can only be applied to faces of actual ‘solid’ models or ‘shell surfaces’. ).

Therefore, within Simulation the relevant tube/pipe (marked “SolidBody#…” under Cut-List) needs to be ‘converted’ to be ‘treated as a Solid’ then the outer face needs to be set with Shell properties before Edge Weld Connector can be applied (note steps below);

1.) In Simulation, under the Part folder > Cut list > Cut-List-Item (# of the member) > “SolidBody #…”(pertaining to the member);
2.) Right click the “SolidBody #…” > select “Treat as Solid”
3.) Right click the “SolidBody #…” > Shell Manager > in Properties window, select the outer face(to apply “Shell”) > below, Select “Thin”(or “Thick”) > for Thickness enter the tube’s thickness/units.

Now the Edge Weld Connector features can be applied to the tube(s) generated with Weldments - Structural Member feature. One might ask then why bother with Weldments - Structural Member feature at all(?), well that is because during the design phase in which dimensions of a frame can be changed frequently, it is much easier to work with sketch lines and auto trim(miter) than generating 3D tubes each time manually when dimensions & angles need adjustment.

Sorry for the long winded reply… 'hope this helps some folks!

And as you mentioned, simplified parts significantly reduce wait time for FEA.

Cheers~!

6

Before you reinvent the wheel, as long as welder follow welding standard, the join will be as strong as base metal if not stronger.
So first ask yourself, why are you analyzing weld join? You don’t have a certified welder? You are not welding to standard? You use new material which not in standard?

7

Good questions Frederick. I understand my comments are no news to a SW/Simulation expert (which I am not). I just wanted to follow up what I started with confirmed solutions to my questions that were not specifically clarified unfortunately (by anyone else).

BTW, I am a certified TIG/MIG welder and can also braze, with some years of experience welding thin walled steel and aluminum tubes, so fortunately I don’t need to find someone to weld for me. My intent in understanding how Simulation processes joints(Contacts/Connectors etc.) is to understand Simulation’s limitations/quirks, so that the stress/strain data of the tubes around the joints can be “taken with a (proper) grain of salt” if you will, in preparation for official tests to bicycle industry standards.

Whether a joint is analyzed as the default ‘Bonded’ type, or as a ‘Contact’(No Penetration) with Edge Weld Connector, the results will be an approximation. In fact, there is no practical way to model a “proper” fillet weld’s “root penetration” profile (fusion beyond the 90 degree joint point into the materials) with any official feature in SW, as around 50% of the thickness of both joined members(in the case of thin-walled tubes) should be fused with the bead forming filler(welding rod/wire) material to form the weld bead(i.e. in a standard fillet weld, the terminated member will have say half its thickness fused with the bead and other member, while the other half will just be in contact with the other member - SW has no official feature to model such arrangement).

Below is an image of a fillet weld I did years ago of a 0.9mm tube(cold-rolled steel) to 1.5mm tube(hot-rolled steel), cut/polished & etched with phosphoric acid, showing the grain type differentiation of parent materials vs weld bead profile - i.e. “root penetration” of the bead into both joined members. Notice that the other side of the terminated member is not fused onto the other member, just in “contact”(i.e. NOT “Bonded”), maintaining its edge and structural integrity as it should.
Cut & Etched Fillet Weld.jpg
This is why SW’s default treatment of “Bonded” for use in analysis of intended welded joints would obviously lead to potentially VERY misleading results (for someone unaware of real-world weld joints, sound or otherwise). I wish SW would model such properly root penetrated beads automatically (as their R&D could certainly apply code to do so)!

I’m none the less grateful that at least Interactions(Contacts) setting to Contact and Connections setting to Edge Weld Connector comes close to ‘simulating’ a fillet weld joint, minus realistic “root penetration” and option to apply smooth concave faces in ‘as welded condition’(not filed or sanded), which prevent stress risers along the “toes” of the weld beads (unlike those of lumpy convex beads or flat faced 45 degree angled beads of the Edge Weld Connector feature which form acute angles between parent metal and the weld bead face along the weld bead’s toes).
Then there is the matter of the HAZ(Heat Affected Zone), which is a factor that will likely not be addressed by SW/Simulation any time soon.

But before I build something that I or someone else might ride at very high speeds downhill, knowing via even close approximations of what is without doubt ‘safe’ is obviously necessary, with no intent to “reinvent the wheel.” Better safe than sorry…

Your interest and input are appreciated…

Cheers~

8

Great, you know what you’re doing.
Mesh size will affect sim results. Generally the finer (smaller) mesh give more accurate results.
Mesh are all triangles, always has 3 sharp points for stress concentration. You will get high stress in some locations. You’ll learn, analysis and ignore them.
If you want to test weld join, model simple 2 parts with weld prep, weld bean (concave, convac, grinded flat etc) and run sim on that. Compare that with what you know.
You can model different zone with different material to test deflection. Stress usually don’t change much with material. Stress is more depends on geometry and load.
Model and run sim on old projects that you know worked. They will show you what the sim can do, what can be ignore, what need attention.

Sim is to supplement what you already know. Not to show what you don’t know.