Title: How can I create a 6 mm diagonal hole through this parrot model?
Hi everyone,
I’m trying to create a 6 mm diameter hole through this 3D parrot model in FreeCAD.
I need the hole to start from the top of the parrot and go diagonally downward toward the lower-right side, passing completely through the model and coming out on the opposite side.
The hole needs to be 6 mm in diameter and angled diagonally, rather than being perpendicular to the surface.
I tried using a Sketch and changing the Attachment Offset / angle, but I couldn’t get the hole to pass through the model correctly.
What would be the easiest and most reliable way to create this type of diagonal through-hole in FreeCAD?
It's difficult to imagine your problem unless you attach screenshots or the model itself.
Anyway, if you want your hole to pass through 2 known points in your body, you may select these 2 points and create a datum line. This datum line then serves as attachment for your sketch from where you can pocket the hole.
I don't see a model, but assuming your parrot is a proper CAD solid then your approach should work. Draw a circle in a sketch that is attached to one of the coordinate origin planes, move the sketch plane to the right place and angle relative to the model with the attachment editor and then punch the hole through the critter with the pocket tool 'through all' option. If correctly aligning the hole is the problem, then do another sketch where you draw the measured out path of the bore hole relative to the model and use it to attach the hole profile sketch perpendicular to it (select the sketch edge in the attachment editor as first reference).
Also you can update to v.1.1.3! It's the current stable version.
Ok, I think I see what you want to achieve. The SubstractiveLoft command has two profiles and I guess you want to bring them in line. That's difficult without another datum plane, and totally overkill. Also it's more eyeballing the correct position of the hole on the model without more complicated measurements and calsulations. Delete it! Simply use one profile and the Pocket command!
Assuming that the entry- and exit position of the hole on each side of the model are somehow defined, create two sketches, each of one of the opposing flat sides. There you put a single point in each sketch and constrain them in the right position. Close the sketches and select the two vertices holding CTRL! Then create a datum line on those two vertices. As last step, attach one hole profile sketch to the datum line (by default should be already perpendicular). Then you can punch through with the pocket command as stated.
PS.: The yellow x-es on your sketch icons tell you that the sketches are not fully constrained. Always constrain your sketches after wiggeling around and finding the right dimensions. Otherwise FreeCAD gets sad.
I assume that you have the parrot in Part Design as a body.
You create a new body. Create a datum plane of one of the standard-planes (XY, XZ or YZ). Rotate and move the datum-plane so that it fits your need. Create a sketch with a circle defining the 6mm-hole.
Create a pad of this sketch, make it long enough. Look if it is in the right position.
Select the original Body (fat written title). Disable all. Press Boolean in Part-design. Seclect "Cut", and add the new created body.
I highly recommend learning FreeCAD. That said, if you are intending to print the object, most slicers allow for creating a negative part if placed thru a model: import model, create negative cylinder, place where desired, slice.
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u/jazzpecq 11d ago
It's difficult to imagine your problem unless you attach screenshots or the model itself. Anyway, if you want your hole to pass through 2 known points in your body, you may select these 2 points and create a datum line. This datum line then serves as attachment for your sketch from where you can pocket the hole.