How do you create your welded constructions?

[torbjorn_heglum2]

In our company we do a lot of tailor made welded constructions. Normally this is based on cut steel plates and beams. Some of the steel plates are bent, and often the weldment is machined after welding. So in principle our design can be a nice mix of functionality found in standard parts, sheet metal, frame generator and a weldment assembly.

However, to work efficient with a welded design we would prefer to work top-down. I.e decide main dimensions and overall functionality before we start detailing parts. As far as possible, we would want the parts to be associative to the main geometry and update when main dimensions are changed.

If all our parts were beams the top-down approach could be served quite well by the frame generator, but unfortunately there are always some lugs, some box constructions or other plates that should be associative with frame members. We could use adaptivity on such parts, but find this approach to unpredictable.

So the most effective way we have found is mulitibody parts – crating one body for each part, then using make components to generate the final parts. Very effective, the derive functionality of Inventor is great. We are able to control the whole assembly from the base part, and all changes are extremely smooth. I have seen base parts controlling assemblies with 100 individual parts, and they still update quickly and it is quite easy to figure out dependencies between the bodies.

With this workflow we have to create all standard beams and profiles as individual features, so there are some extra clicks compared to the frame generator. But the flexibility and rebuild time is superior to the frame generator. Have tried to make standard profiles as ifeatures, with no success due to lack of flexibility and support of multibody parts. And we still miss the possibility to control the machining from the base part – it has to be added un-associative in the assembly.

Note, we are still in Inventor 2014, so there might be some new functionality making top-down design more effective.

So how do you make your mixed weldments – plates, beams and machining? Is there a good top-down approach or is it more common to changes by measure and tweak until fit?

Torbjørn

[Sofia.Xanthopoulou]

Hi @torbjorn_heglum2,

have you ever heard of skeletal modelling? This is often used for Top-down approaches to control an entire construction based on one or two main sketches. YouTube videos with tutorials are available 

Happy New Year!

[JDMather]

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@torbjorn_heglum2 wrote:

.... Have tried to make standard profiles as ifeatures, with no success due to lack of flexibility and support of multibody parts. ....

Torbjørn

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If you continue to use your current workflow - be sure to look into Sketch Blocks for your standard profiles.

[blair]

If you have "Standard Profiles" look at publishing them to Frame Gen as well. Nothing says a Frame-Gen item needs to be a long beam. It can be a beam end cap plate as well.

[torbjorn_heglum2]

Thanks for your reply, Sofia 

The way we work is indeed skeletal modelling, the main sketches controls to some extant all bodies of the base part. Then each body is derived to individual parts and assembled in the resulting assembly. Actually, we also place the base part (the skeleton) in the assembly, as a structure used to constrain duplicate parts. 

This way we try to keep all design intent in one object, i.e we try to avoid design parameters placed in single parts or the assembly if possible. Below you see a simple skeleton, whene the red is reused geometry - used to constrain duplicate parts.

 

But we have not found any good method to control machining from the skeleton. Even if we make sketches for machining in the skeleton part, we cannot import or project anything associative from those to the assembly features. Have found sort of a workaround for this, but too complex for practical use. So we remain to match the machining allowance in the skeleton with the assembly features manually. 

Maybe there are some improvements since inventor 2014, that could link this together?

Or are there any known effective workarounds to control the machining from a skeleton?

Torbjørn

[torbjorn_heglum2]

Thanks for your reply, JD

Yes, we use Sketch Blocks for profiles and some standard designs. As Sketch Blocks can be derived between parts, this makes it possible to create a sort of ‘library’ of Sketch Blocks to be used across different designs.

But ideally, some added functionality in the ifeatures would be a great timesaver, and would also make the browser more tidy. At least for Inventor 2014 the flexibility of the ifeatures are too limited; ifeatures can only be added to existing bodies and separate ifeatures are needed for various termination options.

Do you know if it is possible to create a new body on placement of an ifeature in Inventor 2017?

Torbjørn

[torbjorn_heglum2]

Thanks for your reply, Blair

I see what you mean, it can be a possible way to make the frame generator more usable for us. But there will still be members that would be hard to predefine, as they just need to adapt to the surrounding geometry.

How do you place such members? By adding points (or short lines) in your skeleton, similar as ‘long’ members?

We have designs that will work perfectly with the frame generator, but others are more odd. Like this walkway, it is a nice mix of standard profiles, plates and swept tubes. But to make everything fit, we still prefer a top down approach.

 

Torbjørn

[blair]

I don't think that one single method will work. Looks like some of Top-Down, Middle-Out and Bottom-Up. Frame-Gen for the portion that best suits it as the main structure.

I might use a sketch of the side profile and then extrude it as a Surface model to develop the width of the assembly. Then place sketches on the faces as needed for the Frame-Gen items. Then fill in from there.

[torbjorn_heglum2]

Thank you for your toughts.

As I see it, the multi body approach covers most cases, but not always intuitive and often long browser trees. (To compact the browser tree, I tried to add folders in the part browser via the API, but no sucess so far. The method is there, but it seems to fail for parts). So I guess we just will have to continue to look for more effective ways to do our top-down approaches. 

Still, it is a pity that the ifeatures haven’t been developed more during the years, the functionality is more or less the same as back in 2005. If it just were possible to create a non-failing combined ifeature for a structural member, the workflow could be quite smooth and the browser three much more compact. Some day, maybe…

Torbjørn

[blair]

There hasn't been any changes to iFeatures since they were introduced.

Either "Sketch Blocks" as JD suggested or adding your profiles to the Frame-Gen.

Sometimes, you just need to use all or a combination of the modeling techniques. You post a problem here on the forum and you will get as many differently created models all with the same finished result.

[smokes2998]

If you are using assemblies you can convert the assembly to a welded assembly. I use weldment as it is an SW term.

If you do this you can add prep features to the assembly and machined features to the assembly you must remember you can out remove material with prep features and machined features.

You can do most of the examples in frame generator but i would recommend getting training in it as it is quite convoluted. i.e the work flow make no sense to anyone used to doing weldments.

This is what I would suggest other than switching to another Cad system which will do the job more efficiently and getting training.

[Sofia.Xanthopoulou]

Hi @torbjorn_heglum2,

I understand that it is not easy to clearly define "THE" solution on such a complicated topic. Still there are some good approaches, including your descriptions. In order to let all readers benefit from your experience, please mark at least one post as accepted solution, so they get something like a summary of possible workflows.

Thank you and good luck with your projects

[jtylerbc]

My company's situation is similar to yours, and we use a variety of the tools (in a variety of different ways) in Inventor to deal with it.  I don't think any of these are techniques that haven't been mentioned already, but I'll list some of it to give specific examples of when and how we use those tools.

• Frame Generator:  Obviously, we use this for any sort of a frame. 
• Multisolids:  We often use multisolid modeling for any sort of a plate steel structure.  This allows us to make things "adaptive without Adaptivity".
• Custom templates:  Where multisolids don't seem like the best solution, we have a series of customized part file templates for steel plates, from completely blank except for some property information, to complete shapes with iLogic forms so that you can model common shapes without ever entering a sketch.
• Adaptivity:  Yes, we actually use Adaptivity (carefully).  I'm a little less scared of it than most, although I tend to steer my less experienced users away from it until I think they are ready.  It can be quite finicky, so it needs to be used carefully and sparingly.

The project I am working on right now (sorry, not going to show pictures) is a frame for a piece of hydraulic equipment.  It consists of a number of different pieces, including MC channels, HSS square tubing, and plate steel.  Some of the plate steel is bent to form what is essentially a custom channel.  FInally, there are holes that are drilled post-weld (a very simple case of post-weld machining).

1. The bulk of the frame is modeled through Frame Generator.  The base plate and the bent channels are created using the multisolid technique.  You may not be aware of this, but there is nothing that says that the "Layout" part for your Frame Generator has to only contain lines.  In this case, the Layout is also the multisolid,
2. The bent parts are converted to sheet metal so they can be flattened.  This is only possible in the last couple of Inventor versions.  On 2015 and older you would need to derive those parts into a second part file before it will let you convert to sheet metal, due to the incompatibility between multisolid and sheet metal features at the time.
3. A few plates need to be located from frame members (ex. plates welded to the MC channel).  Since they are not located on the same face that was used for defining the frame member location in the layout, this is a pain to include as a multisolid.  These are simply inserted as normal parts and constrained to the channel and tube parts created by Frame Generator.
4. One of those plates is notched to fit around one of the Frame Generator-created parts.  This was done using Adaptive techniques (using Copy Object and Sculpt).
5. The assembly was converted to a weldment, and the weldment's Machining environment was used to add the post-weld holes.

As others have mentioned, there is no one tool for this type of modeling, and every idea that's been suggested in this thread has a potential application.  Hopefully these examples will give you some ideas how you could make use of the options available.