Good evening everyone, I can't do a circular repetition with the "leave" and "chamfer" functions on solidworks.
I get an error message: "The selected functions could not be repeated using the geometry repeat. Clear the Geometry Repeat check box.
I uncheck the "geometry repeat" box and I get an error message: Can't create an occurrence for the repeat. try again, decreasing the number of occurrences or the distance between the occurrences.
However I can see the repetition in yellow which is valid before validating the action and getting these error messages, there is something I must be doing wrong but I don't see. Thank you for your help.
No problem, I have created a simple document for example as an attachment, I want to make a circular repetition of the leave on the other three edges in this example.
Ah, I wanted to open the file but it must be a 2018 (I'm in 2017SP4).
Indeed I find the same error but the subject has already been discussed here for a linear repetition:
Excerpt from Mick.Cordero 's best answer: This is a limitation of SOLIDWORKS, it is impossible to repeat a chamfer, fillet, or draft alone because these functions are dependent on parent functions for defining faces or edges.
In fact, fillets and chamfers can only work by selecting entities to which they are going to be attached and not in repetition!
It would have to go through a repetition of bodies or other associated functions.
I confirm Antho's answer, SW cannot repeat a fillet or chamfer as a function. When possible, the solution is to use the global symmetries of the part and to apply the repetitions to the whole body, see attached pdf file, and there are never any problems.
Of course, in the case of the example presented, selecting all the edges at once is faster. But often symmetry, or circular repetition, does not only concern a fillet function but other functions of the workpiece. This is what I call the geometric specification, specificities that must be found in the creation tree. If the part is symmetrical, especially only half of it, it is the best way to guarantee this symmetry. Same thing in the case of circular repetition, make it only one sector. If the part also includes smoothing functions, it is essential (positioning of the connectors). On the attached image I only made a very small bit that I repeated as a body.
In addition, working in this way helps to avoid functions that bite each other's tails. A sweep that starts from one place and ends at the same plant often (try a variable gong on a closed 3D edge connecting left faces...). It is better to do it with two separate ends rather than at once. This approach is very valuable in surface for design products that are only splines, nurbs and 3D sketches.
otherwise you can do it by going through a sketch and an extrusion, but it's not very clean... The easiest way is to work on 1/4 of a part if it is symmetrical on 2 planes. Otherwise, use the same function multiple times and match the parameter values of the functions with the equation manager.
SW doesn't really like tangent surfaces in the functions repetitions (fusion), intersection, fusinner, drilling, ... Sometimes you have to chip to the nearest 0.0001 to force the result.
Thank you for your help, in my case I used the solution of ac cobra 427
"Why clutter the creation tree with an additional function when you just have to click on the other 3 stops for the fillet or the chamfer to be done... "
because in my case it was the simplest solution but in a case with more repetition Pierre's solution is certainly the best.
It's a shame that sw doesn't take into account this circular repetition because in my case I had several fillets and chamfers with different angles on several faces (a little more than 10 faces).
On the other hand, with the solution of ac cobra 427, I was able to make several leaves with the same sides by selecting the edges but I could not do it on some sides with the chamfer, the cut was bad.