Designing a steel structure, what are the ways

[alpopkov]

Hello,
I am looking for the best way to design a steel structure. It mainly contains profiles, but may also contain steel plates. The sections of the profiles (2D sketches) are to be stored in Teamcenter, they are customized as a part family. Later, they are assigned to some sort of path. The paths are mainly straight with some curved exceptions.

What is the best way to define the path? (Is routing application possible to use?)
Is it possible to somehow automate the placing (for example extrude sketch along multiple curves at the same time)?
Is it possible to somehow automate the treatment of the profiles in the connection points (for example certain profiles are cut when intersected with another)?
Is there a way to set the connection through some sort of fittings (again, via routing)?
Is it possible to create BOM in the way that it recognizes similar models and makes them the same item?

Please let me know if you can help with any of this questions.
Best regards,
Alexander Popkov.

 

[JohnRBaker]

For more information about the NX Routing products, go to...

http://www.plm.automation.siemens.c...c/routed-systems-design.shtml#lightview-close

...and for a more detailed description of the module, click on the link in the lower right part of the page where it says:

Additional Resources
PDF NX Electrical and Mechanical Routing

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[JohnRBaker]

And even if you didn't go with the 'Mechanical Routing' product, NX provides Rolled-Structural profiles as part of the Reuse Library which can be used to create structures and mechanical frameworks:

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[TheeCircle]

Hi John,

Is that Reuse library in NX9? I was looking in NX8.5 but could not find those profiles.

Thank you

John

 

[PDW]

Hello John,

You need to download the ReUse Library from the GTac website.
I think it can be found under Full Product Dowload.
You need to choose your Operating System
Then you should look for Machine Library.

Hope you can do it with this help

 

[TheeCircle]

Pascal,

Thank you! Works great!!!

John

 

[PDW]

Hello John,

You can also find some interesting Best Practices, this about the creation of ReUse Parts and the creation of ReUse Fastener Assembly.

Kind regards,

 

[SvenBom]

About the original question from Alexander. In short, it can be yes to all your questions.
In mechanical routing, you can draw the lines or select the edges of the model for creating a path. When the path is created, you can place a profile to just one segment of the path, to several segments or to whole path.
The profiles are defined just with a 2D section and control points. With those points, the profile is connected to the path.
At the corners, the profiles are treated with different options automatically.
BOM is also created automatically. You can select, that all the same profiles (regardless the length) are treated as one (thus you get the total length), or you have the position number for each profile (profile with same length have the same position number).

You can create your own profles just by editing the existing ones. Or (better), you can create completly new groups and sections, without touching the defualt ones.

Here is also the link to one of mine previous post on this subject:

http://eng-tips.com/viewthread.cfm?qid=349585

I hope, that this answers your question and that it will help you with your work.

Kind REgards.

 

[alpopkov]

Hi all!
Thanks a lot for help!
I used the Routing => Platform to make the steel structure. The corners are getting done in the correct way with Assign corner option.
Is it possible to cut the "middle" profiles using other profile. I tried to use Assign corner with Cope option, but it seem to be working only in case both curves end in the same point. <
The screenshot is attached.
Thank you in advance!
Alexander.

 

[SvenBom]

After selecting the RCP (routing control point), you have to select both profiles. First, select the profile from the square geometry (outside geometry) and then select the profile from the inside. It should work. I just tested this and it worked for me.

Regards.