Hi all I'm looking to create a repeating countersunk holes on a concave surface. Also, I want each of these holes to be normal to the surface.
Currently, I have managed to make my surface concave, to create repetitions of points on my surface, thanks to the CreatePoints tool from MyCadtools. The idea afterwards was to make a countersunk hole, then to make a repetition by sketch. The problem is that if the axis of the first countersunk hole is vertical, all the holes will also be vertical and not, normal to the surface as I would like. Do you have an idea for my holes to be normal on the surface?
Hello clement.carribon_2, Welcome to the forum hoping that we can help you find the solution. Your request is interesting, I've never tried it. For my part, I would aim to do them in appearance, but I think it's not won. I think someone has a solution. Good luck. …@+. AR.
You should know that, if you select your concave surface and then click on the drilling wizard, the positioning sketch will by default be a 3D sketch → all the points will be on the surface and every drilling will be normal to that surface.
The problem is that repetition in a 3D sketch is inaccessible.
All this to say that, the first option, tedious but perfectly meeting the need, is to manually define all the points in the hole positioning sketch which must be a 3D sketch.
The second is to see whether, from the flat, drilled sheet, the Deform function In curve-to-curve mode, you could get the result you want.
Thank you for your feedback, I need to make this part in 3D printing afterwards, that's why I need all the holes to be represented correctly. Representing them by an appearance will not work in this case.
Indeed, it is at the time of repetition that the problem arises, and given the number of holes I would have liked to avoid placing them one by one, especially if behind you realize that you have to change a dimension for example.
I'm going to look for the distort function. If I can find the desired concave shape, it may be a solution.
Solidworks has a problem with repetitions: it only knows how to repeat with the same orientation... and it's extremely frustrating!
For example, if you make a slotted hole pointing towards the center of your piece and then you ask for a circular repeat: the slotted hole will keep the initial orientation instead of reorienting each entity towards the center
So, the same goes for your piercing, it won't be able to repeat (to my knowledge) while remaining normal to your plan (which is intuitive for everyone here)
The holes must have their " origins " on the surface, and their axes must be normal to that surface. But what about the position of the origins of the holes on the surface? Judging by the image, they appear to be obtained by projecting a 2D grid onto the surface. True or false?
If you have a 3D sketch that contains the center points on the surface, a simple macro can create normal holes in that surface. On the other hand, each hole will have its own sketch to be generated. At a glance, 1250 plans, 1250 sketches, 1250 material removal function. Solidworks will row...
Can you share the SW model of the baseplate with the sketch positioning the holes? Even in degraded form, it would make it possible to test feasibility.
Hello Thank you for your answers, The method of @Silver_Surfer , repeating on a flat surface and then using the curve-to-curve deformation function, is perfectly suitable; You have to remember to tick the " following the curve " option.
In curve-to-curve mode, you could get the result you want.