Exporting a Part for 3D Printing
This document will describe the workflow necessary to export a 3D part in SolidWorks to a file that can then be imported to your 3D printing slicer program.
Two different options / workflows will be presented by examples, and the pros and cons of each will be discussed:
- (Preferred) Export to a STEP file or
- Export to an STL file
Both workflow options will be described independently in sections below.
In addition, tips for dealing with a Part that contains multiple Bodies will be discussed.
Finally, an example will be provided to demonstrate how to re-orient a part prior to export. This can be beneficial if having parts printed by a 3rd party vendor that assumes that the part to be printed will open in the proper / desired print orientation.
Prerequisites required:
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SolidWorks for Makers 2024
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Access to the Input-Inc. CAD repository (The February 2024 CAD Release will be referenced in the included examples)
Older versions of the Input Inc. CAD releases included a '3D Printable Parts' folder with pre-exported STL files. That folder has been deprecated, should NOT be used, and the STL files contained within are very likely out of date!
Do NOT use any pre-exported STL files. Always export the files (to either STEP or STL) yourself!
When exporting a SolidWorks 3D part (.SLDPRT) file for 3D printing, there are two popular files types: STEP (.step or .stp) and STL (.stl).
STEP files are preferred, and here's why:
- The file sizes are much smaller, and
- (most importantly) the original geometry is not modified
However, there is a downside to STEP files: Not all slicer programs currently support them.
So, the decision is clear: if your slicer program supports STEP files, use them!
STL files offer no advantage over STEP files, and actually have a severe disadvantage:
- The original part geometry is modified by tessellation during export!
Yes, you understood that correctly: STL files do not contain the original part geometry. They contain an approximation of the original geometry, and the accuracy of that approximation is only as good as settings you choose: poor approximation/small file size or better approximation/very large file sizes. If you have ever looked at a 3D printed part and wondered why it had facets instead of smooth curved surfaces, STL resolution settings are the culprit!
To illustrate this, here is a comparison of the [TUPR-B-COVR-01] Potentiometer Covering.SLDPRT file in Bambu Studio:
You can see that SolidWorks' default "fine" STL export setting results in an STL file that is very faceted (left) as a result of the tessellation that occurs during export. Custom STL export settings would need to be set in order to achieve a better result (middle) at the expense of file size. Compare that to the appearance of the exported STEP file (right): the file is only 6.4% the size and matches the original 3D part geometry!
Let's use a Part in the updated V2 Neck Drive Assembly as an example, so open the assembly [TUPR-C-V2] Neck Drive.SLDASM located in the \[04 TUPR] Upper Torso\[C] Neck Drive\[V2] Plate Interlock\ folder.
From this assembly, we will export [TUPR-C-V2-COMN-08] PCB Mount for 3D printing. The Part is highlighted in blue in the screenshot below:
Open this example Part by left-clicking it in the FeatureManager Design Tree and then clicking the Open Part icon as shown:
With the part to be exported now open, go to the File menu and select Export As... as shown in the image below:
In the Export dialog window that appears, select a folder to save the .STEP file to, and set the the file type to STEP AP214 as shown below. (The AP214 standard is overkill for this use, but we've seen no harm in using it and it appears to be compatible will all STEP-friendly slicers.)
Click the Export button and you are done. You can now import the .STEP file into your Slicer software and start printing.
We will use the same example Part that we used in Example 1 above, so refer to Example 1, Step 1: Opening the Part to be Exported if necessary to open the appropriate Part file.
With the part to be exported now open, go to the File menu and select Export As... as shown in the image below:
In the Export dialog window that appears,
- select a folder to save the .STL file to,
- set the the file type to STL, and then
- click the Options... button as indicated in the screenshot below
In the System Options - STL/3MF/AMF dialog that appears, set the Resolution to Custom, and the Deviation and Angle tolerance values to the recommended values shown below. NOTE: This will yield large file sizes but with geometry that most closely matches the original 3d part (as discussed in STEP vs STL above).
Click OK to close the System Options dialog, then click the Export button.
You will then be presented with the tessellated STL preview as shown below:
Click the Yes button to save the part. You can now import the .STL file into your Slicer software and start printing.
Let's now compare our Workflow 1 (.STEP) and Workflow 2 (.STL) parts.
We can see that the .STEP file is indeed a much smaller file than the .STL:
In Bambu Studio, the parts look indistinguishable, with no obvious faceting:
Sometimes, a Part file will contain multiple Bodies that are intended to be treated as separate objects... either for machining or 3D printing. One such example can be found in the [TUPR-A-COMN-08] Wire Tunnel part of the updated v2 [TUPR-A] Frame.SLDASM assembly, highlighted in blue in the screenshot below:
Open the [TUPR-A-COMN-08] Wire Tunnel part. This Part contains 2 Bodies that we will want to Export and print separately. If we select the Split operation in the FeatureManager Design Tree, we can see the "cut line" that splits this part into 2 separate Bodies:
Now, scroll up the FeatureManager Design Tree, and select / expand the Solid Bodies(2) entry as shown:
Select the Split1[1] body and it will highlight in blue on the Part as shown:
Now, go to the File menu and select Export As... as shown in the image below:
Follow whichever workflow you prefer (STEP or STL, referencing the examples above as necessary). Two additional steps are required, however:
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Append the file name to be something unique (such as adding "left" or "right" to the file name), as SolidWorks defaults to the name of the Part, not a unique name of the Body.
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once you then click the Export button, you will be presented with an additional dialog window. Make sure to pick Selected bodies as shown below.
Once that Body is saved, select the other Split1[2] body in the FeatureManager Design Tree and Export it as well, again making sure to give the file a unique name.
If performing slicing yourself, it is always possible to re-orient the exported part in your slicing program. However, if you are using a 3rd party vendor to print parts for you, it is always suggested to make sure that the part will be imported by them already in your preferred orientation. This can help avoid confusion, and can be very important in the case of standard FDM printing, where:
- given that the strength of an FDM printed part is anisotropic, and as such it is required that the stronger features (perimeters / wall loops) provide strength in the required directions. In other words, you may need to avoid part separation along the weaker Z-axis / layer direction.
- a part face that is cosmetically important may want to be face-down on the print bed.
- costs can be minimized through proper orientation, minimizing support material and/or the need for post-processing.
NOTE: This procedure ONLY works if exporting to STL! Use only if necessary for a 3rd party vendor.
Let's use [TDRV-COVR-01-L] Shield Covering (Left).SLDPRT as our example. When opened it looks like this:
As an example, we will export the Body named Chamfer3. Go ahead and hide the other 2 Bodies in this Part file to keeps things easy to see:
Now, let's assume we want the outer face (highlighted in the screenshot below) to be down on the bed when printed, to get the best cosmetic surface on that viewable face... and to eliminate the need for support material.
The simplest approach to re-orienting the part prior to exporting is to: 1. create a new Coordinate System that is oriented properly and tied directly to the Body to be exported, then 2. select that new Coordinate System when exporting, to tell SolidWorks to use that orientation.
First, we need to create the new Coordinate System that is oriented properly to the part. To do this, select the Features tab, then Reference Geometry, then Coordinate System as shown below.
The new Coordinate System we will define needs to be pinned to the face we want to be facing up (NOT the face on the print bed!).
The tool presents you with several selections to be made, as shown below:
The Position entry is selected by default, so click a point on the upwards face of the Body. Ideally, we would pick the exact center of the part but it is not critical. Try to select a point that is near the center of the Body as much as possible, as shown below:
A tricolor coordinate system will be drawn at that location:
Then, in the Orientation section of the Coordinate System options, click in the white box beneath Z axis:. It will turn blue once selected.
Now, click on a desired upward face of the Body as shown below:
Finally, we need to make sure that the Z-axis (blue) pointer is pointing in the right direction. It must be pointing directly away from the selected face of the Body, not through the Body. This is the correct direction the Z-axis (blue) pointer must be facing:
IMPORTANT: If the orientation of the blue Z-axis pointer is not correct, click the Reverse Z Axis Direction button to the left of the Z-AXIS selection as shown below to flip it:
Click the OK (green checkmark) to confirm your selections, and the new coordinate system will be created in the FeatureManager tree:
Note: it is assumed here that defining the face to be up when printed is sufficient, such that it is not important to define the other directions. I.e., it is not important that the Front be the front (instead of the Rear or Left) when printed, etc.
With the new Coordinate System defined, we are ready to export our part.
Go to the File menu and select Export As... as shown in the image below:
Select STL as the file type, and enter a unique file name to save as.
Then, click the Options... button:
In the System Options dialog that appears, click Export in the left column, then under File Format select your intended file format, and then finally select the Output coordinate system as shown below:
Click OK to close the System Options dialog, and then click the Export button to export the STL file.
Note: when you click the Export button, you may be presented with an additional dialog window. If so, make sure to pick Selected bodies as shown below.
If the exported STL is now opened in a slicer program, we can see our specified orientation is correct, with the intended outside cosmetic face down on the print bed:
