CAD Translators 1

[jrmartin]

Our department has begun making the switch from IDEAS to Solidworks. Our license agreement with IDEAS runs out this summer.

Has anyone any experience translating from IDEAS/SDRC to Solidworks? There are a few packages out there that claim bi-directional capability for solid models like Elysium. Can translators handle drawings?

OR, should we just hire a summer student?

Your feedback is appreciated.

 

[Beggar]

My (limited) experience is that you're generally better to recreate models if they're something that you continue to work with. I've had some success translating models but have generally found you end up with fewer headaches and a more robust end result by starting from scratch.

I'd hire the summer student...

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Bring back the HP-15

http://www.hp15c.org

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[ctopher]

I'm not familiar with what format you can save as in IDEAS. I suggest find out what format you can save that other CAD software can import (in your case SolidWorks) then start saving all of your existing files in IDEAS to that file type. Save them in a folder for legacy. When you do not have IDEAS operable anymore, you will have your files available for other programs. You can then hire someone to do the translations for you or do it as you work on them. Good luck

Chris
Sr. Mechanical Designer, CAD
SolidWorks 2005 SP0.1

 

[jrmartin]

To research this, I tried using FEATUREWORKS in SW2004 SP4.2 to convert a dummy solid into extrudes, revolves ... natives in general. It seems to be successful about 60% of the time.

When it's unsuccessful, the natives which did not convert seem obvious to me. I try to convert them manually (opposed to automatic recognition) but they still are unrecognized.

QUESTION: Has FeatureWorks been improved in SW2005?

TIA

 

[TheTick]

IDEAS translators are tough to come by, not nearly as common as those for CATIA, even.

For translation service, I highly recommend MathData Services <

http://www.mathdata.com>.

They got all the toys and will translate and inspect and clean up. Input and output in most CAD and neutral formats, incluing SW and IDEAS.

I could be the world's greatest underachiever, if I could just learn to apply myself.

http://www.EsoxRepublic.com

-SolidWorks API VB programming help

 

[VicDude]

jrmartin,

You are in deep. I have been involved with what you are trying to do for many years. There are no true "bi-directional" translators for what you are trying to do. At best you will be able to end up with a dumb model (no history tree) and a non-associated 2d drawing. The best conversion from IDEAS 2d to SW 2d is by processing your IDEAS 2d out as cgm files, reading them back in, and then posting them back out as dxf files to be read into SW. You end up with only vector information, text becomes lines and arcs, but atleast what you end up with is an exact vector replica (no clean-up). For the 3d, did you try posting the model out as a parasolid and then reading it into SW? If you are going to try and send a 3D assembly model, it is going to translate as the last saved configuration in IDEAS. So, you will want to make sure that your asy's and sub-assy's are in the configuration you want. The rest of your configs are lost.

Hope this helps.

 

[jrmartin]

Thanks for your drawing solution. It sounds like MAJOR work, especially for 1000's of drawings. At this point I think we'll keep 1 seat of IDEAS for emergency purposes and convert as necessary.

Yes, I tried parasolid. It provided the same dummy solid as an IGES conversion. Is there something I'm missing? Also, IDEAS would only parasolid out a part, it wouldn't handle an assembly.

TIA

 

[VicDude]

You can do the 2d conversion in a batch mode mode with a simple script. Print out to CGM, open CGM, save as dxf. You can also write other commands into the script, such as changing layers or line types, color by entity types, etc. This way you can do an entire project from TDM at one time or all the projects. The computer does all of the work for you. We translated over 13K files in less than two weeks. They all ended up as what you saw is what you got.

To do the 3D assemblies from the IDEAS assembly environment, you do this:
File menu - Interoperate - find and pick the assembly file - save it as a parasolids.XT file - go to where you saved it and open it SW.

You can also write a script to batch out all of the parts or assemblies in a porject. (NOTE: parts come with assembly exports)

 

[SBaugh]

Look at

http://www.capidia.com

- Format works2005 - You might want to call about that one.

Also look at

http://www.elysiuminc.com

I pretty sure they support IDEAS. I was just talking with them this past week at the SWWC.

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
faq559-716 - SW Fora Users

 

[nsessions]

I'm just thinking out loud here:
Isn't Solid Edge NX/IDEAS/UG "lite" in a similar manner that SW is to CATIA? Wouldn't EDS or SDRC have a format that will commute between the two? and aren't SW and SEdge in a similar price bracket? just a stab in the dark ... but you see where i am going?
/n

 

[Cadbotte]

VicDude,


I have to make a choice which format to use when picking the assembly file? ex UGNX
And the type sets to unigraphics xpk which can not be changed back to parasolid.XT. When I pick on a part file I have no problem making an parasolid.XT. What am I doing wrong with the assembly file?

Is the parasolid.XT file better convertet into SW then an iges file made with SW-flavour?

"To do the 3D assemblies from the IDEAS assembly environment, you do this:
File menu - Interoperate - find and pick the assembly file - save it as a parasolids.XT file - go to where you saved it and open it SW."

/C

 

[VicDude]

CadBotte,

The XPK (package) file is the file that UGNX and Solid Edge interoperate with, and what UGNX to UGNX from two different installations (not networked) transfer back and forth. They retain the relationships within UGNX.

You want to use the parasolid file over the IGES file only if your models aren't created with a lot of surface commands, because SW is utilizing a parasolid kernel for modeling. I would recommend using IGES translations for complex surface models, because you can flavor the IGES better.

I have to check my notes, but I belive (will verify) that you can't bring an assembly model, with all the parts separated, using IGES.

To quote nsessions, "I'm just thinking out loud here:
Isn't Solid Edge NX/IDEAS/UG "lite" in a similar manner that SW is to CATIA? Wouldn't EDS or SDRC have a format that will commute between the two? and aren't SW and SEdge in a similar price bracket? just a stab in the dark ... but you see where i am going?
/n"

FYI - SE has a translator just for IDEAS, because they are both UG products. They are not made for bi-directional interoperability though. I have translated IDEAS to SE, and it works well, and keeps the rework time to a minimum.
VicDude