importing from Mechanical Desktop to SW2004

[PhilLee]

Hi guys,
I need some advice regarding importing files from Mechanical Desktop to SW2004. I'm not positive what version of Mech Desktop it is but it would be one of the latest, if not the latest.

I have tried using .iges but I end up with the model simply as a imported body and I can't edit the sketches.

1) What format do I ask for the Mechanical Desktop files to be saved in, and
2) are there any tricks when opening them in SW.

Best regards,
Phil

 

[CorBlimeyLimey]

Whatever format you get from MD will be imported as an "imported body" ... without sketches ... by SW. The "trick" is to use the FeatureWorks add-in if you have it. This will recognize features & create sketches that SW can work with. It, almost definitely, will not reproduce the features, in the same sequence or type that were created in MD though.

Your best bet would be to obtain a variety of formats (STEP, IGES, Parasolid) to see which is imported & recognized with FeatureWorks the best.

from (the City of) Barrie, Ontario.

Everyone has a photographic memory. Some just don't have film.

 

[SBaugh]

It doesn't matter what you import, it will always either be an imported body or a surface body. Either way you don't get sketches to work with. It a dumb solid that's it. You can try Featureworks if you have it. It might recognize some features, but I have not seen it do a great job in recognizing imported bodies.

The way I look at importing is: Parasolid (1), then STEP(2), then IGES(3), finally ACIS (4).

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[PhilLee]

Scott,
Is there a difference when importing a part vs an assembly? Will the assembly be one solid body or will SW recognize it as seperate parts?

When you have to edit a part that has been imported, can you simply draw the sketch over the body, then change the dimensions etc.. Will the imported body 'follow' the new sketch? Or is it simpler to recreate from scratch?

Thanks,
Phil

 

[SBaugh]

s there a difference when importing a part vs an assembly? Will the assembly be one solid body or will SW recognize it as seperate parts?

It's going to vary depending on how it was exported. If it was exported as an assembly Then you will probably be importing it as an assembly and get separate parts. They will all still be imported bodies or surface bodies.

When you have to edit a part that has been imported, can you simply draw the sketch over the body, then change the dimensions etc.. Will the imported body 'follow' the new sketch?

You cannot edit an imported body and no it will not follow the sketch. THe sketch is a child of the imported body.

You draw sketches and add to the imported body. But it will not change the imported body.

Or is it simpler to recreate from scratch?

That's going to vary on it's complexity. But if you need to change it and Featureworks doesn't recognize (or you don't have it) then you will probably have to recreate it.

At least you have a 3D model to take measurements from. You could start a sketch on the imported body and convert the edges. Then once you complete the sketch, you could simply copy it from one part to another. You might have to adjust it (Tools\Sketch Tools\Modify), but the sketch is there.

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[JimSym]

If you have MDT and SolidWorks on the same system, you can do a feature-based conversion and end up with a fully editable assembly. Works quite well.

 

[Fortyplus]

As JimSym points out if you have MDT on your system then use the supplied Converter native to Solidworks. Its not part of FeatureWorks.
I have used this converter to convert our MDT5 files to SWX2003.
I've found the convertor will hang if you are converting some Assembly models and I tend to resort to just converting parts only then build the assemblies in SWX.
Also Note that the XY planes are 90 degrees different to each other so rectangular arrays get skewed.
You also get lots of planes.

 

[DesignSmith]

If you can get the MDT and the SolidWorks on the same station, using the DWG import will automatically recognize the MDT files and run MDT in the background to import them with features. Should you run into a problem assembly in that arrangement, try converting the major parts first, then doing the assembly again.
If the files are prior to MDT 4, open-regen-purge-save, in MDT 5 or 6 before converting. (numerous cases of bad geometry from prior version files)
Otherwise, set the ACISVER system variable as high as it will go in MDT, then use the ACISOUT command to give you new *.SAT files that can import nicely into SolidWorks.

DesignSmith

http://www.DesignSmith-Services.com