buick455 wrote:Still have the Regal to this day, just wish it aged as well as I have, lmao..
buick455 wrote:BTW I'm 6of1 over on the RR boards.
RR = RepRap?
Just got one myself not long ago (an AO-100 from Lulzbot, which is a MendelMax 1.0/1.5 clone with the build volume of a Prusa)
buick455 wrote:& my attempt in FreeCad so you can see my progress
The problem with your model is that you have made 4 separate, non-connected pads. They are actually 4 separate parts. But this is not what you want: you want a single cube-like object. The way you did, you'll need to do a boolean fuse to join them together.
This is not necessary in Part Design. First, think of the Part Design workflow as if you were machining a solid block with a milling machine. You start with something big then cut away stuff. Of course sometimes it's better to add material, it all depends on the shape. But for prismatic parts, you should not need to use boolean operations, because the features deal with them for you.
Second thing to know: once you have your starting feature (usually a Pad, but can be a revolution too), to keep working on this solid, you need to map your sketch to one of its faces. Mapping a sketch to a face is the process of linking this sketch to the face of a solid. It is easily done: just click on the face on which you want your sketch to reside, *before* creating the sketch. Otherwise, you will get the Plane selection dialog, which means your sketch will not be linked, and you'll be starting a whole new part.
Mapping a sketch to a solid's face also allows you to use external geometry (edges of the solid) as reference.
buick455 wrote:Getting things constrained is for the lack of better terms a pain in the butt
Well the more complex your profile, the more constraints you need to apply - so yes, it can be tedious. Which is why I'm a big proponent of Breaking the Modeling Down into Small Chunks™
. (I didn't trademarked it, though I should!
) In my experience it's often faster to create many simpler sketches and features than a single complex one with a single feature.
Another tip: use geometric constraints as much as possible.
And finally, do not draw in a sketch what you can add as a feature later. I'm thinking about fillets, chamfer, and transformation tools (pattern, mirror). Those are very useful for holes and repeatable patterns.
Replicating your example, here's how I did it:
My first sketch is a single rectangle, centered on the origin (0,0).
The rectangle is centered on the origin point with the symmetric constraint. I selected the top left point, then the bottom right point, then the origin point before applying the symmetryt constraint.
Next I pad it to 47mm, then I select the front face:
Then I click on "Create new sketch". This maps the sketch to the face of the "Pad" feature. Now I draw the cutout:
Here I used the
External geometry tool to copy the vertical edges of the face. This creates magenta-colored lines which are non-editable. I draw a rectangle, and apply dimensions referencing the magenta lines' endpoints. This will ensure that even if I change the first sketch's dimensions, the cutout will always have specific widths from the side and top edges of the box.
I close the sketch, then I click on the Pocket
tool, and I extrude it by 50mm. Here's the one weakness of this method: This is one parameter which I cannot relate to the outer box depth. If I change it, I'll have to manually edit the Pocket depth.
Looking at the Project tree, I now have two features: Pad, then Pocket:
Pad was automatically hidden once Pocket was created, because Pocket is the "child" of Pad. Both are representations of the same object
. When working on a part in Part Design, the tree is a history of creation of the part, showing the sequence in chronological order. Pocket is now the current state of the part, and we should continue work on this feature, not on Pad. Pad should stay hidden and not be worked on, unless we want to edit it or its sketch.
Next I make the top cutout: I click on the top face of "Pocket", then I create a sketch in a similar method as previously:
I close the sketch, then I create a new Pocket 5mm deep. This creates a new "Pocket001" feature and hides "Pocket".
Next I select the bottom face of Pocket001 and create a new sketch to pocket the centered hole. The current feature is now Pocket002.
I select the bottom face of Pocket002, and create a new sketch. I'm now planning to cutout the four 1.5mm radius holes, but I only draw one circle in my sketch!
I drew it in the top left quadrant but I could have chosen any of the 4 locations. Again I close the sketch, then I pocket it - this time, through all. That's right, I want it to punch through the top recess. More on that later.
The latest feature is now Pocket003.
Here's the fun part: patterning the hole I just pocketed. Since I made sure the rectangle in the first sketch was centered on the global origin, I can use the Polar Pattern
feature. I select the Pocket003 feature, and click on the PolarPattern icon. I leave Angle at 360 degrees, and set Occurences to 4. The preview should look like this:
That's a lot faster than drawing and constraining all 4 circles in the sketch isn't it!
After clicking OK a new "PolarPattern" has been created in the tree which now looks like this:
Next, I select the top face of the recess and create a sketch to pocket the large hole. The process is the same as for the bottom centered hole. I end up with "Pocket004":
Now I select the recessed face of "Pocket004" and create a new sketch for the angled rectangular slot. The reason for punching the small hole through is revealed:
I'm using the external geometry tool again, this time to copy the edge of the small hole. (It does not copy the whole circle, but rather an arc. This is one of FreeCAD's quirks.)
I can then add tangent constraints from the linked arc edge to the long edges of the rectangle. I set a 135 degree angled constraint from an edge of the rectangle to the horizontal (red) axis. And to center the length of the slot to the hole, I draw a small line from the center point of the copied arc edge. I do not attach the other end to the rectangle side yet, and click on empty space. I apply a symmetric constraint between the two endpoints of the rectangle's long edge, and the small line endpoint. This automatically centers the end of the short line to the rectangle's edge. Then I turn the short line to a construction line, and I add a perpendicular constraint between both lines. Here, only one dimension constraint was necessary, for the length of the rectangle - its width is determined by the hole diameter.
Almost finished. I make sure Sketch006 is selected and pocket it, this creates "Pocket005". All that is left to do now is to create a second PolarPattern based on Pocket005.
The end result is this:
That's it! Of course there are other ways to do it, but at least you have an idea now what's possible.
Don't hesitate to ask questions if you need clarifications.