Hi all,.
In toolbox of solidworks we have structural steel option.
when i m clicking on the structural steel option one pop up window will come & in the drop down menu only
ISO
ANSI
BSI
CIS
DIN
JIS
are coming .
as we have some our customize sections (tailor made) so please tell me how i can add them to above given list.......
so we can perform the beam calculator option on that...
thanks in advance
RAVI
Solidworks 2009 Professional SP.3.0
Dear tom,
u r correct but after following ur method my custom profiles are added to the structural member option of the weldments toolbar....
but i want to add these profile to the toolbox---> structural steel option..
Hi Ravi,
As far I know, you can only edit tool box items through 'Configure' toolbox interface. In order to do this you have to go to ( while any SW file open or creating new file) menu toolbox -> configure.
You will see this configure toolbox interface.
1.There, by selecting one of the standard, you can copy that standard to update with your custom changes.
2. Once you copy your custom standard, you can go down until your required toolbox item (here, structural members), lefthand side, you can add size you want to item you want as shown in my screen shot. You have to have all dimensions of the member in order to create a new size.
I think this is the only way to customize your toolbox if you want do all your beam calculations...etc.
Hope this helps.
Regards,
mkp
SW 2008 Pro, SP. 5
XP Pro, SP. 2
Attachments
Dear Krishna,
After following your procedure we are able to add our custom profiles in the Toolbox.
But we want to add these profiles in a dropdown menu of beam calculator's Structure steel.
For more details, I am attaching the following pdf.
Thanks in advance.
Attachments
I was attempting to do this as well. I wanted to add Chinese standard (GB) beam sections to the listing in the beam calculator. VAR support responded that it is not possible. The beam calculator (as well as the profiles defined there) is an integrated yet standalone functionality that is not customizable. The confusing part is that it is listed under the "Toolbox" menu option but is NOT part of Toolbox.
I may supplement the dimensional information in a derived GB Standard within Toolbox to include beam section properties for reference. That might be a suitable workaround for me.
My biggest problem with derived standards in Toolbox, though is that when Toolbox is updated during a SP install, derived standards are left alone. So if they add a bunch of data to one of the standards, it does not get added to your derived standard, potentially forcing you to use both depending on what you need. Messy.
I am relatively new in SW and am intersted in this dicussion thread: Did it ever come to a final conclusion?
My interest is to modify / customise the sections available - in toolbox / structutral steel - with global variables which describe the profile section and the standard reference (ISO...) which I can then use in a BOM of the assembly of the various steel profiles
Thanks
Hi Francois,
Where you have the structural member files stored create a new folder called for example 'my sections'.
In part mode create a new sketch of the structural profile making sure its fully defined.
Exit sketch, select sketch from feature tree and go save as, then save as type 'Lib feature part', then browse to new folder and save.
This should then be available for you to use.
Also look under Weldment in the help files and search for 'creating a custom profile'.
Hope this helps
Mark
Though it might be OT but feel it can be helpful if you want to use Weldment way:
How to create Weldment Profile
Add more Weldment Profiles
Thanks to both Mark and Deepak for the suggestions
As I said I am finding my way in SW (convert from Inventor) and I am trying to define the best methodology for weldments involving both structural members and other parts and how to produce a table on a drawing that gives details of profile, length, material, standard and so on. Tabel could be a "Cut Table" of a BOM. The debate is then whether to use assemblies or weldments, both of which have their advantages and disadvantages.
Weldments are multibody parts - no exploded views - designed for standard profiles: the adding on of cut plates and so on can be done by using extruded bosses with manual descriptions to appear in the cut list. What I have also found that patterning these features confuses the cut table.
The workaround is to make the structural steel framework in weldment and then insert it into assembly in which the other plates and objects are added: A 2 level weldment
Alternative is to use an assembly - nice exploded views - and insert structural steel profiles: There are 2 ways of doing this.
- from toolbox in the feature library - parts into an assembly
- from toolbox toolbar - structural steel - sketch into a part.
The former is easier to create parts in the assembly, more demanding both to position them and to link lengths to global design changes (though I have yet to work out how "layout" works)
The latter lends itself to the use of a "skeleton" part with one 3d sketch of the framework as a derived part in each structural member: Sweep the profile along the relevant line in the sketch. Change the skeleton changes all the structural members
I have a liking for this approach, but for this I would like some more intelligence is the base sketches : global variables describing section and so on, a point at the centre of the profile ....
Hence my question
Thanks again