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A flywheel with a diameter of 230mm shrinks to 2.45mm when exported as dxf file
ProApe
Member Posts: 52 ✭
Hello,
I have drawn the linked flywheel with a diameter of 230mm in 3d, converted it to a 2d drawing with the aim of milling it, and exported the drawing as dxf to do so.
When I open this dxf in Estlcam, the program I use to create the GCode, it has a diameter of 2.45mm!
2 questions:
* what am I doing wrong? Is that the right way to export for milling?
* can I generate the GCode directly in Onshape?
With kind regards
0
Comments
This is a copy of your document, look for sketch 8 and right-click export dxf.
You could have done this part with 1 sketch in the beginning and build the part with several extrude's
I have followed a tutorial where the author created the object with as many sketches!
There are many ways to get to the same end geometric shape. The tutorial you followed was not created in a very efficient way, but in the end, it got the desired shape.
The shape of your model is a 2.5D (CNC terms) shape, or 3D (CAD terms shape). A shape like that is typically exported as a solid model STEP file from the cad program into the CAM program. Why are you using dxf, which is a 2D export? 2D export such as dxf is typically used for laser cutting and waterjet. CNC such as a milling machine or a CNC router almost always uses a 3D STEP file.
Next, if your CAM program really does want a 2d dxf, then you must make sure it's full scale. If you export it from a drawing (meant for paper printing), you must do a few things. First, delete all the drawing border/title block/rev block/dimensions/centerlines, etc. There should be nothing on the sheet except the lines of your part. Next, make sure the drawing is set to 1:1 scale. You currently have it as 1:4 scale. Next, dxf is a dimensionless format. When you go from program to program, the second program does not know if the first program was in mm, cm, inches, etc. You must tell the second program what the units are.
If you want to avoid all that, you can do what Dirk did in his sketch 8 of your model, and export the dxf from the 3d model, rather than the 2d paper drawing. (although the units will still have to be set in the second program).
For the second question, no, you can't create g-code natively in onshape today. CAM is in the pipeline for later this year.