exported STL without chamfer

[sanzo]

Hi all,
Finally I got to use FreeCAD for something useful
I modeled a broken piece of my washing machine (too old to get spare parts) and I'm trying to get an STL file to send it to a 3D printing service.
The problem is the exported STL file doesn't have any chamfer, but if I try to export only the "Chamfer" object it exports fine.

link to an image that explains the problem
Is there something wrong in my model? How can I solve this problem?
Thanks for your attention!

OS: Mac OS X
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.16.6321 (Git)
Build type: Release
Branch: tag: 0.16_pre-osx
Hash: da4e6ccd624dbfcf8dc49282ab67951f989ba63c
Python version: 2.7.11
Qt version: 4.8.7
Coin version: 3.1.3
OCC version: 6.8.0.oce-0.17

[cox]

Your part consists of 4 individual parts, by using theTools:dependency graph you can visualise your projects interdependencies.

Screenshot_20160430_143147.png (16.77 KiB) Viewed 1882 times

In your case I guess you could select all 4 parts in treeview and export or select all 4 parts and Part:Fuse them together and export while only the fuse is selected in treeview.

[sanzo]

Thanks cox, it worked!
I didn't know I could fuse more than two parts (I should have RTFM!). I previously tried to fuse the parts in pair and then fuse the two fusions, but the result was the same as before. Now I can finally repair my washing machine!

Thanks again,
have a nice day!

[cox]

Good luck, glad it worked

[NormandC]

Hello sanzo,

I modeled a broken piece of my washing machine (too old to get spare parts) and I'm trying to get an STL file to send it to a 3D printing service.

That's one of the best use of 3D printing IMHO. I'm fortunate to own a 3D printer myself, but I haven't used it in 2 years.

I checked your file, and if you don't mind, I have a few tips I'd like to suggest for your next project.

The Sketcher's main purpose is to be used with the Part Design workbench. There is no harm in using sketches with Part tools (or even other workbenches), but when using PartDesign features you can benefit from a work flow that seldom require using Boolean operations.

The idea is to select a face on the last feature before creating a sketch: this maps the sketch to the face and allows you to build additive (Pad) or subtractive (Pocket) features to your model.

I've reworked your file using this method and attached it here. Also, I ordered steps so I only needed to sketch the T-slot once. This allowed me to work with simpler sketches. I don't like to work with complex sketches, they take more time to fully constrain.

The model shows a dependency graph with a single linear branch:

PezzoLavatrice_normandc1_dependendygraph_01.png (47.29 KiB) Viewed 1863 times

The last operation was created in the OpenSCAD workbench with a Refine shape feature. This feature removes unnecessary edges from planar faces.

One advantage of using mapped sketches is that you can link to external geometry, like I did in Sketch004. In my dependency graph, you can see that two arrows point to Pocket001: one of them indicates that there is one linked external geometry in the sketch.

One important drawback of this method is that due to an inherent weakness of the OCC modeling kernel, such models are more fragile and prone to breaking after edits.

A few other tips regarding constraining sketches:

• You sometimes use the length constraint where an horizontal or vertical distance constraint would have been preferable. The length constraint should only be used sparingly, for diagonal distances as it is more taxing on the solver.
• Use as few dimensional constraints as possible. For example, in Sketch each of the circles has a radius constraint. You could have avoided one of them by setting an equal length constraint between the circles. This equal length constraint can also be used between straight lines.
• It is best to limit the use of symmetric constraints. When there are too many in a sketch, they tend to confuse the solver. When it happens the sketch elements lock up and it's almost impossible to find all the remaining degrees of freedom to fully constrain the sketch. If you look at the revised Sketch in my file, you'll notice that I only use a single symmetric constraint between diagonally opposed points. I ensured the symmetry of the profile with multiple equal length constraints.

[sanzo]

(sorry for the late reply, my email subscription rules seems to be broken...)

Hello sanzo,

The idea is to select a face on the last feature before creating a sketch: this maps the sketch to the face and allows you to build additive (Pad) or subtractive (Pocket) features to your model.

I totally need to RTFM!
Thanks a lot for your suggestions, I'll keep them in mind the next time I'm going to model something else!