Nice model. Lacks color though!
Right-click on an object and you have a few choices to change an object's appearance:
- Set colors: allows color mapping of individual faces
- Appearance: set the object's display properties (viewing mode, material, transparency and line width)
- Random color: don't trust your taste in colors? Let FreeCAD choose for you!
yoshimitsuspeed wrote:Actually this is the most complex thing I have ever drawn as a single part. I'm so used to the ability to make something as an assembly I never had to try to do this.
The fact there are no 3D relationship tools yet does not preclude creating an assembly in FreeCAD. One just has to translate and rotate the parts manually, or create them at the right position to start with. Of course there will be no relationships between the parts, it will be kind of a "dumb assembly" like you would get from SolidWorks by exporting to .x_t (Parasolid) or STEP format. But hundreds of thousands of designers and engineers over the world have been creating assemblies in AutoCAD that way for a long time. (of course this figure is a wild guestimate, as probably most AutoCAD users only work in 2D)
The only thing to know at the moment, is that for parts created with PartDesign, it's the first sketch's placement that you need to change. If you attempt to move the part itself it will reset to its original position. This is because the "Body" feature is not implemented yet. As I understand it it is a container for all features in a part. It will also make it easier to differentiate the parts in the Project tree.
yoshimitsuspeed wrote:The edge link tool is definitely still rough around the edges. Sometimes it works well. It usually links fine to the last thing in the design tree and or whatever you are sketching off of. Other things it just won't recognize.
The edge copy tool will only work if the sketch has support, i.e. is mapped to a solid's face. And it will only recognize this solid's edges and no other. If this happens to be a feature, it won't recognize previous features of a same part. Some type of edges it does not support, like splines. Yes it is limited, and will surely be improved in the future.
yoshimitsuspeed wrote:Several times when I tried to pad the sketch it just disappeared. If I moved the sketch or made a pad that contacted the sketch the pad feature would often work.
I am not sure I understand what problem you have. It would be useful to post a file to demonstrate the problem, so the developers can find out what's wrong and fix it. In fact I find this very odd because the pad feature has worked very reliably for me for a long time. I have never seen a sketch disappear: not produce a solid, yes; but this happens if the profile contained in the sketch is not closed.
FYI the PartDesign workbench aims to create single-body parts. At the moment, to ensure a pad feature fuses to an existing part, the sketch needs to be mapped to a face on this very part (by selecting first the face before creating the sketch). If it is not, the pad will create a new part separate from the other one. What you need to do then is to fuse them with a boolean union from the Part workbench. Of course there are cases where you won't have a choice but to do that (for example have a hole go through a cylinder) But this will be addressed in a future version of FreeCAD, hopefully the next release (v0.14).
yoshimitsuspeed wrote:For example the pads that hold the outer rails. I made the sketch referenced to the outer surface of the box. If I try to pad them to go outside that they disappear, If I reverse direction and pad them inward they work fine.
I don't understand. If you try to pad them to go outside what? What is the plane the sketch resides on? Is it on the box's side?
yoshimitsuspeed wrote: I made the rails just smaller than the hole and they wouldn't pad. once I made the rail slightly larger than the hole so they were in contact they padded just fine.
Yes, as I said, the single body rule. What you could do is not map your sketch to the pad, but on an independent plane. Then you create a separate part which can have a smaller diameter. Of course, then the copy edge tool won't work.
BTW there is a topic where we share our creations (Show your FreeCAD projects here!
), it would be cool if you talked about your project there and posted your pic. Since I did not want to clutter the other topic with our discussion I did not merge your post to it, but it would be a good idea to link to your topic here.