Parasolid

If you create a part from an inch start part, it should import correctly and retain the system of units. Just don't open the .x_t directly; instead, do 'Insert>Shared Data>From File' and copy in the geometry from the parasolid file as you first feature after the datums. Opening directly defaults to meters, even if it started out in inches. I've exported inch stuff to parasolid, opened it to check how the export went and found that the export converts units and it imports as meters.

I have tried that but what I found is that when the parasolid is a assembly it does not see the different details. And when you try that with a assembly start part it converts back to metric. Let me know if you have worked with importing parasolid assemblies maybe I might be doing something wrong.

Thank You

David Janes wrote:

I have tried that but what I found is that when the parasolid is a assembly it does not see the different details. And when you try that with a assembly start part it converts back to metric. Let me know if you have worked with importing parasolid assemblies maybe I might be doing something wrong.

Thank You

David Janes wrote:

Hey camtd,

Without an example part it is hard to say whether or not this "fix" will work. Try adding the config.pro option:

pro_unit_sys=ips

This options specifies the default system of units for new models. It may work with imported ones too.

Hope this helps.

--Adam Joseph Cook, Mechanical Engineer

Hey camtd,

I think I figured it out (I tested it on a parasolid part that opened in MM when I tried it at first and when I applied this "fix" it opened with default units "IPS"). I am using Pro/Engineer Wildfire 2.0 M190 over here so these instructions are for this version, but should work in all the Wildfire versions (1.0, 2.0, and 3.0).

1) Create a new part file (*.prt). At the new object dialog name the part "parasolid_template" and UNCHECK the "Use default template" checkbox. Click "Ok" button. At the next dialog that appears ("New File Options" dialog), select "Empty" and click the "Ok" button. Also ensure that the checkbox "Copy associated drawings" is UNCHECKED.

2) Set the units of this new part via Edit->Setup. When the Part Setup menu manager appears select "Units". At the "Units Manager" dialog, set an appropriate system of units where INCHES is the primary unit for length (I recommend the 'IPS' unit system). Select the "Close" button and then select "Done" on the Part Setup menu manager.

3) Save the part file. Copy the part file into a permanent directory (i.e. C:\\templates). However, ensure that NO SPACES exist in the FILE PATH to this part file!!!!

4) Repeat steps 1 thru 3 above for an assembly file (*.asm).

**At this point you should have "parasolid_template.prt" and "parasolid_template.asm" (WITHOUT the version number at the end, i.e. parasolid_template.prt.1") in a permanent directory without spaces in the file path**

5) Set the following config.pro options:

intf_in_use_template_models=yes

template_solidpart=Options... GUI)>

template_designasm=Options... GUI)>

**NOTE: If you have Pro/E started and you add these template files to the "templates" directory while Pro/E is running, you need to restart Pro/E in order to browse to these files"**

6) Apply the options.

**NOTE: Applying the above options will automatically make parasolid_template.prt and parasolid_template.asm the "Default templates" at the "New" dialog when creating parts and assemblies, respectively. You can still use other templates, via unchecking the "Use default template" checkbox.**

7) Import the parasolid part into Pro/E.

8) Hopefully it should work, mine does. I measured the part just to make sure after I imported it.

I hope this is what you are looking for. If you want e-mail me a sample part and I'll try it out on my system.

Hope this helps.

--Adam Joseph Cook, Mechanical Engineer

Hey camtd,

I found an easier way to import geometry into Pro/Engineer with a unit system of your choosing. I don't know if anyone is interested anymore but I thought I would just put this out there.

1. Open your startpart or startasm (the startpart and startasm should have the units desired).

1. Goto Insert->Shared Data->From File...

2. Select your IGES, STEP, Parasolid...etc. part from the "Open" dialog that appears, click "Open" button.

1. A new dialog will appear (most likely in the lower right-hand corner of the screen) prompting you for the coordinate system to which to place the imported geometry. Select the desired coordinate system and choose "OK".

The imported geometry should now be part of the startpart with the correct units. No need to set any config.pro settings for this one.

Hope this helps.

--Adam Joseph Cook, Mechanical Engineer

Always and thanks.

Works for parts, not for assemblies?

Hey Jeff,

I believe that it will work for assemblies in the same way as in parts just start out with a startasm that contains the desired units and datum planes. The Shared Data... option is still available. I would think any IGES and/or STEP file that contains an assembly would be imported as a assembly of parts.

Hope this helps.

--Adam Joseph Cook, Mechanical Engineer