One (the?) solution is to scan a volume body (which represents the diameter of the cutter).
Then you have to be able to adjust the orientation of the tool along the scan (its center must always pass through the axis of your part): there are options for this and you should not hesitate to make different tests.
Be careful, the tool (volume body) must cross the trajectory. You also have to start at the beginning of the trajectory (not the most practical of times).
I tried on your part but I didn't manage to do this removal of material (even taking only the beginning of your trajectory as a spline). (Maybe because of the beginning of the sketch).
Try the much simpler room/trajectory volume body scan feature to practice.
Nb: another solution is to sweep a straight line to make a surface and use the surface to remove material. It works but will be less accurate (does not manage the possible tailgating of the tool). in PJ the result of this solution (not good because the scanned surface is really bad in terms of its geometry)
The solution by scanning a volume body proposed by @froussel must be suitable, provided, as he indicates, that very caution is taken. The idea is to use the future cam roller to generate the surface (or the cutter if the profile is machined). The trajectory curve It must be continuous, without angular dots, which excludes segments. A 3D spline "fitted" on your segment series does the trick, making sure to give it a wide enough tolerance to smooth out any local bumps due to your point-by-point definition of the profile (Tools > Spline Tools > Adjust Spline). The Swipe Tool It is a cylinder (image of the future pebble) whose basic sketch is a circle - tangent to the trajectory curve, - coincides with its origin, - the normal to the plane of the circle from its center must intersect the axis of the cam (Axis 1). Respecting these positioning properties requires the construction of a few plans and sketches... Finally, the volume body scan function generates the surface. The result seems to be in line with expectations... The model is attached, SW 2020. Kind regards.
The only problem in your solution is that your cam is tilted towards the center which is a single point if I saw correctly. @m.blttook care to remove it by wedging the cam on a plane that remains parallel to the axis of rotation. Thus the cam always rises and falls perpendicular to the central axis. I'm in SW2019 so I can't open the room to see his proposal either :-( Sniff !!
But as the cam is always only a single point of contact with the cam raceway, it is enough to make a rectangle perpendicular to the central axis and remove the material swept using the correctly dimensioned spline and provided that any hollows in the cam raceway have a radius greater than the diameter of the cam ;-)
Anomaly: the method I proposed in my previous message does not work... The surface generated is not that obtained by machining by means of a milling cutter driven in a rotational movement around Axis 1, with an axial displacement law given by Sketch3D7. The principle still seems correct to me, but the realization by SolidWorks is not good. This can be seen by making sections of the part by a plane containing the Axis1.
On the other hand, there is a function in SolidWorks that answers the problem (subject to validation, I am becoming cautious...). This is the Winding function (Inserting > Functions > Winding). It allows you to wind a sketch on a surface, and to generate a volume in relief (embossing) or in hollow (debossing) on the basis of this winding. The major advantage of the method is that the "cam" part of the coiled sketch corresponds exactly to its law of lift, i.e. y = f(teta), to a "Radius" coefficient. It is no longer necessary to construct this law of survey point by point, as was the case in Sketches14 and Sketch3D6. Disadvantage: it is necessary to have a cylindrical face of the volume function type at the base, and without holes, chamfers or other details in the winding area. The winding does not operate on the basis of a surface cylinder. On the other hand, the "rolled" sketch should not spill out of the surface. Another consequence: you have to remove the basic cylinder function if you only want to keep the cam path. And only work on the details after the cam has been generated. Model attached, with a profile resembling your original but totally invented + video confirming the correct definition of the profile.
Congratulations to @m.blt for being able to design the piece.
For the anomaly he points out, it is probably due to the non-use of the "specify a direction vector" option (you have to select the axis of the part here). For me the resulting part seems to be OK with this option activated (except at one end where the spline is too short so SW does what it likes at this end).
See the PJ
NB: the AC cobra solution also seems to be OK but the final geometry seems slightly different from mine. This may be due to the tool's tailgating present with my method and non-existent with his (but the gap seems too big for this to really be the case).
A big thank you, for your answers, I was sick last week, now I'm better, I've started to test the solutions.
I have to do 2 cams I tried to do the same operation again but it's not easy, I just have to modify a point of the spline (if you look it is missing the last point of the spline which is not attached) and the scanning function of the volume body no longer works
I'm going to test one element at a time and I think I need your advice to be able to reproduce the function and understand how it works
I offer you a summary of the different answers given to the question asked by @criss, about an axial cam. The conclusions are based on my tests and need to be confirmed. Or contested...
The sheet metal version seems to me to be the simplest and most reliable given the general shape of your part. In the attached zip, your adapted model and some explanations on the method used...
Thank you, for your answers. You have a very good level. For the moment I'm trying to get the right dimensions on the cam on the middle of the cam it's good but on the sides I can't get the real dimensions measured between 3D and 2D Here is my mobile number see private message I use whatt's app
If one day you need me for a gear, maybe I could help you
It seems to me that this is only feasible with a linear trajectory, an infinitely small cam or like the usual cams that generate the elevations at precise rotation angles (not on the whole trajectory).
I totally agree that the profile of the cam and the displacement of the center of the roller that will come into contact with it in a mechanism are two very different things... When designing a mechanism, the transition from a specification that imposes a law of motion to the geometry of a cam that will allow it to be obtained is sometimes a difficult problem, depending on the structure of the mechanism. To get back to our sheep, the question asked at the base concerns how to generate the cam path with SolidWorks, knowing its profile curve, unrelated to the future mechanism and its roller. We are of course on the geometric definition of a room.
There may have been an ambiguity in my remarks, coming from the expression "law of lifting" that I used, instead of "curve of the cam profile". It is true that the first has a kinematic connotation, which is reminiscent of the movement of the roller and its support mechanism, while the second only concerns the geometry of the cam. Mea culpa, my tongue forked without my knowing it.
And to be completely complete and to go in your direction, my "check" of the profile using a mechanism was done with a zero radius roller, precisely so that the cam profile and the lift law coincide exactly.
Can you help me, I have a problem on the 3D winding my create a slope of 5° to the eye on my machined part
I looked at the 3D, there is indeed a winding defect, it creates a face with a slope, see the attached files
I think Lynk's work is great but I didn't manage to modify his drawing because the elements used table etc are much too complex for me, and at first glance visually the shape of the cam does not conform to the physical model part so in my opinion I should modify it is a point table that I don't know how to master too complex for a person of average level.
So I did a swept winding on my base shape but the surface is not straight but leaning inward on the 1.31°
