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When importing geometry from another system, there are times when errors will occur. This can be due to the method that the other system used to write the file, the way SolidWorks® reads the file, or an incompatible feature or type of feature within the neutral file. A neutral file is one in which a vendor will write their native CAD file data so that another vendor can read it. An example of this would be IGES. The focus of this article is what to do when the files don't come in cleanly and how they can be fixed.
While there are many different import formats supported by SolidWorks, the following should be noted with data exchange files:
- Use native SolidWorks files whenever possible
- If the other system is Parasolid®-based, use the Parasolid format
- Depending on the other system, you may want more than one neutral file (IGES and STEP) when working with a new customer or supplier. This would be done for troubleshooting purposes when the neutral file does not convert correctly
There are additional third party direct translators available from our Solution Partners if you deal with a specific type of system on a regular basis and would like to use native files instead of neutral files to exchange data.
Importing the data
There are a number of different types of neutral files that can be used to create SolidWorks documents. Some of these types can be used for drawings (i.e,. DXF™, DWG), and others are suited to parts or assemblies (i.e., IGES, STEP, etc.).
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| Figure 1 – Import file types |
To import a neutral file, select the Open icon or select Open from the File menu. Then select the desired neutral file type from the Files of type pull-down menu. There is an Option button that displays the dialog box shown in Figure 1. These are the file types that can be imported into SolidWorks.
If the data file is just a surface, don't bother selecting the Try forming solid(s) option. This will save time during the import. Also, if you are trying to fix a file, it may be desirable to have the geometry imported as surfaces to look for problems and resolve them on the surface data. The option Do not knit makes each surface its own entity. This will also make it easier to edit the data in the surface file.
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| Figure 2 – Import Option dialog box |
When SolidWorks cannot knit the imported file into a solid, it will warn the user. The solid will have an error flag shown next to the imported feature or the solid will not knit and a surface feature will be shown. SolidWorks will try to fix bad import geometry during the conversion process. If that is not successful, the following steps can be taken.
#1 – General steps for importing and fixing a neutral part file
- Import the neutral file with the Try forming solid(s) option turned on
- If there are errors, review the report file to find out where the neutral file was produced and what problems were reported
- Use the Check Entity function to determine where some of the problems are located
- Use the Import Diagnosis function
- Close All Gaps
- Use the Fix Face function to remove any bad face identified within the Faces field or by the Check Entity function
- If this does not work, go to #2
#2 – Surface import with no sew
- Import the neutral file with the Try forming solid(s) option turned off
- Use the Check Entity function to determine where some of the problems are located
- Use the Import Diagnosis function
- Use the Fix Face function to remove any bad face identified within the Faces field or by the Check Entity function
- If this does not work, go to #3
- If this does not work either, save the file in a neutral format (Parasolid, IGES, etc.) and go back to step #1
- Or select all surfaces and knit them and create a solid using the Thicken function
#3 – Remove and fix faces
- Import the neutral file with the Try forming solid(s) option turned off
- Use the Check Entity function to determine where some of the problems are located
- Use the Import Diagnosis function
- Use the Fix Face function to remove any bad face identified within the Faces field or by the Check Entity function
- Remove the faces that cannot be fixed and put them back in using remaining edge boundaries. This can be done during the Show Gaps evaluation. This function shows, and selects the open boundaries. When using this function and the desired edge (gap) boundary is shown, open the Fill function and the boundary is preselected
- If this does not work, go to #4
#4 – Round-trip the neutral file
- Import the neutral file with the Try forming solid(s) option turned off
- Save the file using a neutral format (Parasolid, IGES, STEP, etc.)
- Go to step #2
- If this does not work, go to #5
#5 – Where to go from here
- Try a different type of neutral file if available
- Look at one of the native file data translation partners
- Contact your VAR
Report file
When a file is converted, a report file is generated. This file is the import file name with an .rpt file extension. When problems occur, review the results file to see more information about where the file was created and where the problems occurred.
*****************************************************************
SolidWorks Corporation - IGES Report
*****************************************************************
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General Inforamtion
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Sending System Product I.D. : Part.SLDPRT
Receiving System Product I.D.: Part.SLDPRT
Sending File Name : F:\Sw\Part.IGS
System I.D. : SolidWorks 2001 by SolidWorks Corporation
Preprocessor Version : Version 5.3
File Creation Date : 010627.073149
Model Creation Date :
Units : IN
Model Space Scale : 1.000000
Author : user
Organization :
=================================================================
Entity Processing Information
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Surface(s) successfully created.
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Precision analysis of IGES file:
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Most prevalent number of significant digits: 6
Highest number of significant digits: 10
Average number of significant digits: 5.7382
Maximum distance to origin: 39.3701
Minimum distance to origin: 0
Effective number of significant digits: 10
=================================================================
Entity Summary
=================================================================
-----------------------------------------------------------------
Type Name Count Converted
---- ---- ----- ---------
100 Arc 22 22
102 Composite curve 62 62
110 Line 81 81
120 Surface of revolution 11 11
124 Transformation matrix 11 11
126 Rational B-spline curve 162 162
128 Rational B-spline surface 18 18
142 Curve on a parametric surface 31 31
144 Trimmed parametric surface 29 29
314 Color definition 1 1
_________________________________________________________________
=================================================================
Import Options
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Include surface/solid entities: YES
-Try forming solid(s): NO
Include free point/curve entities: NO
=================================================================
Result Summary
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SolidWorks Feature Type Count
----------------------- -----
Solid Feature(s) 0
Surface Feature(s) 2
Curve/Sketch Feature(s) 0
--------------------------------------------
Start Time: Wednesday, October 30, 2002 20:27:22
Finish Time: Wednesday, October 30, 2002 20:27:27
Total Processing Time: 0 days, 00 hours, 00 mins, 05 secs
Check Entity
The Check Entity tool can be used to identify bad import geometry. This is a valuable tool for reviewing problems with the geometry prior to either having it fixed or manually fixing the bad import geometry. By default it only looks for invalid faces and edges. Typically, this is the information needed to troubleshoot a bad import file.
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| Figure 3 – Check Entity dialog box |
When problems are identified, they are displayed in the results list as shown in Figure 3. By selecting the error, an arrow appears on the geometry showing the face or edge. This information can then be used to fix or remove that face or edge.
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| Figure 4 – Check Entity result list |
Import diagnostics
There are many problems that can occur when importing geometry. The Diagnostics function can be accessed by selecting the feature, pressing the right mouse button, and selecting Diagnostics. There are three main areas within this feature: Gaps, Faces, and Geometry.
Gaps are used to show open areas within parts. These open areas can be a source for problems. The Next and Previous buttons are used to step through and identify each gap. The gaps are identified with an arrow. Close All Gaps can be used to have SolidWorks try to close the openings automatically. A solid part will have no gaps.
The face section has two options, fix and remove face. The fix face option is the automatic function where SolidWorks will try to fix the problem. The remove face option would be used to remove the problem and then manually go back and insert a new face. After the face has been removed, a gap will be left in the part. The gaps section can be used to identify and select the boundary of the gap. If the face is on the outside of the part and has edges that are not coincident with other edges, they should be created and disassociated from the original geometry prior to removing the bad face.
Simplify geometry can be used to remove redundant geometry, repair bad geometry and topology, simplify parametric geometry into analytic geometry, and reset tolerances. An example of this would be when a planar surface can't be selected for sketching.
Conclusion
The main issue with data translation is that the original system writes a neutral file and then SolidWorks interprets that file. The type and quality of the information varies from system to system. The techniques described in this article can be used to help troubleshoot issues with these files.
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