I'm wondering if anybody has prepared the solid edge file of the Formula 24 kit car for 3D printing? We're hoping to print a 1:12 scale model of the chassis / wheels etc with our proposed body design on top.
I've read some general guides on the process and am willing to give it a go myself / make available to the community if none exists already.
Solved! Go to Solution.
Ok, my initial post was made in ignorance of how tricky this could be!
So far the main obstacles:
Making the model in to a seamless mesh
Scaling the model to 1:12 while maintaining correct wall thicknesses for the 3D printer
First attempt: I removed parts of the model like the wiring, leaving the main details (frame, suspension/steering & wheels). On exporting it as an STL, Solid Edge helpfully informed me that the parts relationships would be broken in the new file.
And sure enough:
Looking again at the save dialogue box SE advises using Revisions Manager to fix this issue. I've searched for info on RM and tried using the program, but it doesn't seem like it would help with saving STLs with the parts in the right position (I could be wrong).
The pic also shows there are a lot of nuts/bolts etc that won't be relavant to include in the scale model. It appears the easiest way may be exporting the steel frame and suspension only, then make simplified wheels etc from scratch.
Will keep you guys posted!
[Any advice or corrections greatly appreciated.]
Here is how I would approach this:
1. Dont worry about the links being broken as this is always the case when exporting from Solid Edge native file format.
2. You will need to scale each rapid prototype part individually and the only way to scale is upon import, so in the top level assembly, show the chassis only, File -> save as Parasolid (.x_t), don't hit the save button yet, click the options button next to the Save button and check Export displayed only. Then okay, then save with the components name (i.e. F24 Chassis). Do this for all components that you want to rapid prototype and give helpful names.
3. For each component you exported, you'll need to import them into a new part file using Insert Part Copy, which is the step where you can specify the scale. Do this for each part you want to scale in their own part files.
3. For the chassis scale model, I would delete the inside wall of the tubes, so all the tubes are solid. Your 3D printer may have the option for converting the insides of these tubes to honey comb to decrease printing time.
4. Once all your scale models are ready, export them to STL files.
Let me know if you have any questions and I can make a video of this later today if that would help.
Thanks a lot for your reply, I will have a go at this tonight when back from work. For step 3 - is that done using Revisions Manager?
All the best,
Hi, you could try the following steps:
Save the assembly as: *-X_T
Open: *-X_T as *.PAR
Create a new PAR
Insert *.PAR as Copy
Now you could SCALE your file!
Revision manager isn't needed during this process.
Simply start a new part file, ensure you're in the ordered environment, and click the Part Copy command (see image below).
After clicking this command, a dialog will open for you to select the part you want to "insert", so choose the file you want to scale and/or alter to prepare for 3D printing. Once the file is selected, click Open and then you can set your scale (see image below). 1/12 scale is .083 or 8.3% of the actual size.
Let me know if you have any other questions.