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Problem with associativity in assembly (by Kunericch)
First of all thanks for creating this software.
Part-Design very nice. I really like it.
But I despair on using constraints in assembly design.
I have built some constructions in SolveSpace and have got more red screen as ever seen in my live.
The same (very simple) constraints at similar construction made in Alibre or Inventor work fine.
Could it be, that constraints in solvespace are too restrictive when the computer makes (very small) rounding errors?
Part-Design very nice. I really like it.
But I despair on using constraints in assembly design.
I have built some constructions in SolveSpace and have got more red screen as ever seen in my live.
The same (very simple) constraints at similar construction made in Alibre or Inventor work fine.
Could it be, that constraints in solvespace are too restrictive when the computer makes (very small) rounding errors?
(no subject) (by Jonathan Westhues)
The solver is not perfectly robust in all cases, but the constraints in your assembly might also be genuinely inconsistent or redundant. Please post your example (including both the assembly files and the parts), and I can take a look.
Assembly (by Kunerich)
Hello
Thank you for your reply.
Attached an assembly with two pats and an .txt with some question.
Thank you for your reply.
Attached an assembly with two pats and an .txt with some question.
(no subject) (by Jonathan Westhues)
In SolveSpace, all geometry must be exactly constrained, with no redundancy. For example, it's an error to constrain the length of a line twice, even if the two lengths are equal. "Symmetric about workplane's vertical axis" already implies "horizontal", so it's an error to apply both.
When you say "At scetch of triangle i can give length of 0.00mm from line for subtraction", are you referring to g007 in part 2? The extrusion has one degree of freedom, the extrusion depth. Point-line distance constrains 1 DOF, but point-on-line in 3d constrains 2 DOF. (For example, a point starts free in space. Point-line distance constraints it to lie on a surface (a cylinder), but point-on-line constrains it to lie on a curve (that line).) I'd recommend a point-face distance or point-on-face constraint there, which always constrains 1 DOF and will work as you expect.
The "normals in same orientation" constraint fully constrains the orientation of a part, because that's what it's specifically designed to do. If you want to constrain two normals parallel, but still permit twist about the normals, then you can use a parallel constraint.
The "hide/show" options in the text browser window apply to (selectable and constrainable) lines and curves in a group. To hide or show the solid model, check "suppress this group's solid model".
The assembly example that you sent appears to be working correctly. Part 2 has one remaining DOF, and will be fully constrained if, for example, a single point-on-face constraint is added.
Some other CAD programs permit the user to overconstrain geometry with no warning, as long as the constraints still meet certain tests (e.g., redundant but not inconsistent). SolveSpace does not, and I suspect that accounts for most of your problems.
Let me know if you still have trouble.
When you say "At scetch of triangle i can give length of 0.00mm from line for subtraction", are you referring to g007 in part 2? The extrusion has one degree of freedom, the extrusion depth. Point-line distance constrains 1 DOF, but point-on-line in 3d constrains 2 DOF. (For example, a point starts free in space. Point-line distance constraints it to lie on a surface (a cylinder), but point-on-line constrains it to lie on a curve (that line).) I'd recommend a point-face distance or point-on-face constraint there, which always constrains 1 DOF and will work as you expect.
The "normals in same orientation" constraint fully constrains the orientation of a part, because that's what it's specifically designed to do. If you want to constrain two normals parallel, but still permit twist about the normals, then you can use a parallel constraint.
The "hide/show" options in the text browser window apply to (selectable and constrainable) lines and curves in a group. To hide or show the solid model, check "suppress this group's solid model".
The assembly example that you sent appears to be working correctly. Part 2 has one remaining DOF, and will be fully constrained if, for example, a single point-on-face constraint is added.
Some other CAD programs permit the user to overconstrain geometry with no warning, as long as the constraints still meet certain tests (e.g., redundant but not inconsistent). SolveSpace does not, and I suspect that accounts for most of your problems.
Let me know if you still have trouble.
(no subject) (by Jonathan Westhues)
Oh, and to be clear, it's fine to underconstrain sketches. It's just never okay to overconstrain them, regardless of whether the result is inconsistent or just redundant.
assembly (by christian faudais)
hi
a few day ago , i have made a small movie , perhaps it can help you
http://www.youtube.com/watch?v=J2udPIMtmJ0&feature=youtu.be
bye
chri
a few day ago , i have made a small movie , perhaps it can help you
http://www.youtube.com/watch?v=J2udPIMtmJ0&feature=youtu.be
bye
chri
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