This blog is a compilation of frequently asked questions pertaining to the DXF/DWG Import Wizard and DXF/DWG importing and exporting options.
Q: What is the reason that a DXF file with 2D/3D sketches might import with sketch entities when imported into a SOLIDWORKS Drawing, but not have entities when imported into a SOLIDWORKS Part?
A: This may occur if the DXF file doesn’t contain “Mode Space” data, but has “Layout Space” data.
To work around this issue:
- Open DXF file in DraftSight.
- Activate layout space > drag to select entire entities > copy
- Activate “Model Space” > Paste > save DXF file > Import it in SOLIDWORKS Part.
- Open new part in SOLIDWORKS > drag and drop DXF file in part > DXF entities are imported as block.
Q: Is there a better method to centering a DXF/DWG drawing sheet when using the SOLIDWORKS DXF/DWG import wizard?
A: If the two options or the “Center in sheet” selection do not work to your satisfaction, cancel the importation and perform this test: Open the DWG/DXF with DraftSight, zoom out so the drawing will be shown very small in the graphics area, then hit Ctrl A. If new gripping points appear, the drawing may have extra entities that could cause a centering problem.
The DWG/DXF file can be treated prior to the importation using either of two command line methods, this first method using the Purge command, and the second using the Wblock command.
Q: Is there a reason why some entities might not be shown in the DXF/DWG import preview?
A: This can occur if the position is not fully fit into the screen. Perform a zoom to fit to see all of the available geometry. In the DXF/DWG import dialog, select the zoom to fit from the preview toolbar above the preview window.
Q: Is it possible to predefine import units in the SOLIDWORKS DXF/DWG import dialog box so a user can bypass manually setting them with each import?
A: In the registry there are no settings as such for predefining the import dialog box units. Users need to specify them manually in the DXF/DWG import dialog box.
Q: What are the steps to export and or import blocks to or from an external DWG file in AutoCAD?
A: To export a block to an external DWG file in AutoCAD:
- Use the command ‘wblock’ (write block) and browse to select the path and DWG file name.
- Import the block from an external DWG file in AutoCAD.
- Use the command ‘insert’ and browse to the DWG file name with the block definition.
Q: Why might the ‘Align sketch’ command not function when I import a DXF/DWG file?
A: The ‘Align Sketch’ command only works if the ‘Automatic Solve’ function is active. When you import DXF/DWG files as sketches, the SOLIDWORKS software can disable the ‘Automatic Solve’ function for performance reasons.
To enable the ‘Align sketch’ command in a part file that you create from a DWG file, do the following:
- Edit the sketch.
- Go to ‘Tools’ > ‘sketch settings’ > click on ‘automatic solve’.
Q: When using the Task Scheduler to import DXF/DWG files, is it possible to specify a custom scale for resulting SOLIDWORKS drawings?
A: Unfortunately, the task scheduler user interface does not provide the ability to scale DWG/DXF files during for import.
This still may be possible using the application programming interface to create a macro and then, using the task scheduler, run the custom task.
Q: Why might dimensions not comply to changes after creating sketches from DXF/DWG import drawings and adding dimensions?
A: This occurs because the automatic solve option under tools > sketch settings is set to off. To make it comply, set the automatic solve sketch setting option to on.
When DXF/DWG imports have many elements, the automatic solve option turns off automatically. For reference, the automatic settings of the automatic solve option affect the number of points that control elements. Number of points refers to the starting and ending points of straight lines, and the number of control points in splines.
Q: How are endpoints connected, that are not merged in a DXF/DWG file, imported to SOLIDWORKS as a sketch?
A. In SOLIDWORKS after importing:
Note: the merging point value in the DXF/DWG import wizard is a range that within its distance, end-points will be merged.
Edit the sketch entity and apply the repair sketch if necessary (click tools > sketch tools > repair sketch). Review the SOLIDWORKS help module “repair sketch” page.
Prior to importing: Use the PEDIT command on the *.DXF file (type or pe at a command: prompt) prior to importing it into SOLIDWORKS. The command options include; close, join, spline, Ltype gen, and undo.
Application Engineer | CSWE
Computer Aided Technology, LLC