I have a model that I originally modeled in Solidworks but I now what to import into Solid Edge. I have both the SW part file and a step file made from the SW part file.
My issue is that the model keeps coming in as a series of part copies and not body features or another solid model form. How can I convert these part copies to body features?
I would move them to Synch, then on the construction bodies, right click and Toggle them to Design body.
I opened your file and all the bodies are Design Bodies, so they are all solid. Where do you want to go from here? Keep in mind that if you want to add features to a particular body, you must activate it (expand Design Bodies node and double click on the body needed or right click on geometry and select Activate Body) as you can only add features to the active body. You can Synchronously edit them all at any time.
Like Ken I would have to question what it is you are trying to achieve and what your expectations are. Everything appears to be as should be with the file import.
My only comment would be is that this appears to be an assembly, do you want this is as a single model file or do you want an assembly file with individual .par files for each component? Having each component in its own file will simplify your workflow as you then don't have to use a multi-body workflow. However, there are also benefits to having an assembly in a single model file, mainly around file management.
Lastly, as this is an import, you have the ubiquitous blue circle with an "I" icon on each part copy. You will need to run the Optimize command first before you attempt to start modifying and working on each of these bodies.
Bruce, this question is addressed in GTAC Solution Center article 002-7007119.
I have cut and pasted the article below for everyone’s convenience.
Blue circle "i" symbol
After importing 3rd party files into Solid Edge there is a blue circle "i"
symbol shown on the imported features. What is this symbol and what does it
This blue circle with an "i" symbol means you need to run the Optimize
command because the imported geometry has not been optimized.
Some of the downsides of non-optimized geometry include:
Window display performance:
* Slow window updates such as zoom or fit
* View rotations may be slow and jerky.
* Abnormal display problems (Missing faces)
* Problems adding or removing material (cuts/protrusions)
* Direct modelling failures (unable to move face)
* Crashes or abnormal finish to a commands
Draft Drawing view creation or updates:
* Unable to create drawing, section, or detailed views
* Update view fails, hangs, or takes an abnormally long time to finish
What the Optimize command does:
"Increases the precision and quality of the model by simplifying B-Surface
definitions, heal edges, and identifies and replaces blend like faces with
a PS rolling ball blend."
From the Solid Edge Help documentation:
"You can use the Optimize command to increase the quality of the imported
model by simplifying B-spline definitions and healing model edges. Even if
the model does not contain faults, it is always good practice to run the
Optimize command since it improves the precision and complexity in most
If you ever see the blue circle with an "i" symbol, please take the time
to run the Optimize command.