Hello everyone,
A piece must have a 60° angle. The whole thing is inclined and parallel.
Despite this, it doesn't line up because a difference in angle appears.
On the 60° square, the dimension of 60° is measured on the edges and the dimension of 60.84° is measured on the faces of the same angle.
So the interface, which is 60° long, doesn't align.
Any idea?
Hello
Looking at your .jpg the green piece does not fit the gray part in the lower part, is this normal?
Fred
Hello
Same as Fred, on the other hand if you want both sides to follow you just have to edit the dimension of your folded part in the assembly and do = then click on the dimension of 60 so they will be linked.
You also have to check how you have side your parts with the decimals because I think you have displayed the sides in gray and the other one is side in the assembly.
"inclined and parallel": I have trouble perceiving the thing.
If the angle is 60° between edge and another Enter Face value, it means that the plane of measurement of the angle between edge is not the plane with the greatest slope (see with my remark above).
Can you provide your documents?
Looking at your image, I suggest you check the flatness of the interior surfaces of the angle, if there is not a certain slope.
Thank you all for your quick answers.
In the attached image, you can see what I mean by tilted and parallel.
I specify this because the problem does not arise when the assembly is vertical, i.e. the parts constrain each other very well.
No flatness problem and 2 decimal places each.
"The green room does not fit the gray part in the lower part, is this normal? "No, and that's precisely the problem, since they are 60° every 2.
Try to tie the ribs together to see if it changes anything, and if it does change you'll have to see if you can post a Zip with your pieces so that we can take a look,
Given the system, there is a "stupid" problem of constraint which means that the pieces do not follow each other according to the position.
Put your files (asm+2prt) online so we can take a look at them.
You make a take-away composition (or pack'n go depending on the version of SW), it will suggest you to make a zip, when you make your answer, below the input window there is a browse button to get your zip.
Or posted your 2 pieces separately
to test your assembly
There is everything in the assembly, it also happens to me from time to time to design everything in the assembly and then to record the parts one by one afterwards...
The problem comes from the position of your Sketch1 of your T0 extrusion because the sketch is not parallel to your profile. Look, I did an extrusion on the other side parallel to the profile and the angle is good. To correct the problem, you should create a plane perpendicular to your Sketch3D1 and extrude on both sides. I just projected the sketch on the plan and when you measure it there is 60.84°, you would have to put on my plan your Angle 60° - 110 x 7 for it to work like in my room 3...
I can't open/download your assembly, I only have one page of code.
I chose this extrusion method because it's the only one that allows me to have cuts at the ends of my profile without going through the Adjust tool which is a bit cumbersome to manage.
And I remember now that I had the same stress problem with a round tube pylon.
If the tube is a welded construction (square ends) the concentricity stress works well with another round part, if it is an extrusion (horizontal ends) the concentricity stress does not work and I had solved the problem with the collinearity stress of the axes of each part.
Wouldn't that be a small flaw?
In any case, thank you for your indications.
To download the assembly just right-click on it and save the link as... Once downloaded, you will understand that it is only because your sketch is not perpendicular to your 3d sketch that gives the direction... And if you do it to the next side you will also have screw cut from the edge...