Here is the file:
The cable is Ø 1.5 mm
noyau_a_usinage_2.sldprt
Hello @LeStef,
I was able to replicate your problem at home. On the other hand, your sketches were not totally constrained (presence of blue lines, a dash in front of the name of the sketch) and some sketches failed to be rebuilt because they did not find the sketch plan.
It's usually a very good practice to properly constrain sketches.
By redoing them, I exceeded your 100 mm mark (cf. pj.).
M.
noyau_a_usinage_2-2.sldprt
Indeed it's better, but unfortunately the count is not there...
Here are examples of what could correspond to the request
See attached image
The part was made via scanning with circular section
after surface offset and thicken
SW 2017 attachment to optimize .............. (this is only for the principle)
@+ ;-)
parcours_pour_cable_chauffant_sur_cylindre2.sldprt
@gt22
With this method, two separate solids are created. It is impossible to merge the thickening, or to combine the two bodies.
On the surface the geometry is good, but the junction of the two bodies appears, and it is impossible to make a section of the part (in 3D and in the drawing).
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Hello @LeStef
You're never satisfied...; -).......; -)
Everything in its time
you asked how to model this part it's done
yes there it is in multibody
if it doesn't go well for your haircut
you have several walkthroughs
1- Save your piece in another format
(parasolid or step)
and reopens via SolidWorks for testing
2- Take all the surfaces you sew and form a volume
yes sometimes you have to know how to juggle with the log
and on this piece your sweep is quite heavy
but that's another question
@+ ;-)
Never happy ;-)
Let's say that I was hoping to find a robust solution, so that I wouldn't need to fiddle around the weaknesses of Solidworks...
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After all, it's a question of value for money
It is also possible to create the heating cable passage profile
via surface smoothing by creating X sketch along the path and x guide curves
we go a bit + far
in surface when volume
that you can transform into a volume
and via a Boolean operation of removal of matter on the receiving body
but it's a little longer ;-)
It is also relevant to put a + 1 to the right of the answers that allow the Schilblik to move forward
@+ ;-)
Hello.
If I understood correctly, the fct you make should be successful, like a letter in the mail.
Can you send me your part file in SW? I'm going to try a few things.
It's easier than redesigning everything myself.
Thank you.
Hello @fminisini
By rereading the replies posted
you will find the posted files
so you can download them
@+;-)
Hello fminisini,
The initial file is available on page 4 (sldprt) and 5 (parasolid).
The thickening file:
noyau_a_epaississement.sldprt
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Hello
Is the problem solved?
If so, can we have the file!
Kind regards
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Hi @Zozo_mp
For my part, I think I have given an acceptable solution to the question asked
the file under SW 2017 is attached in one of my previous answers
The fact is that it is multibody
Possibility of transforming it into a single body
with reworking of the seam surfaces and forming a volume
@+ ;-)
@gt22. Yes, not bad. However, I have the impression that in the loop, the shape of the throat section is not constant, it varies a little. But it's ok visually and to pass cables.
On the other hand, I don't understand the point of creating an offset surface and then thickening...
Why not create a larger cylinder diameter right away...
It's the removal of sweeping material that imposes a circular section, right?
It's a pity that we can't impose an oblong shape instead of the circle. We would make the throat deeper and directly on a larger diam.
Thank you in any case for this information.
I think the problem is rather how the groove will be made in the machine. If it is in CNC, the machine will reproduce the defects which are not annoying in themselves since it is to pass a cable.
On the other hand, if we make over-quality by having a perfect groove (as for a grooved cam, then the part must be perfect in SW.
We should understand why there are these imperfections????
Kind regards
Unable to find a way to make the entire impression with a single function, I went back to my previous method by refining the junctions.
Process Description:
Cylinder Ø14.6 mm length 410mm
1 - Sketch of the U-turn trajectory
2 - Winding the sketch
3 - Sketch of the shape of the imprint
4 - Removal of swept material (trajectory + guide curve)
5 - Setting up a helical curve of 12mm pitch from the previous cavity.
6 - Removal of material swept by a volume body of the shape of the impression
7 - Same thing on the other side
That's it!
The junctions are correct:
End of story!
@LeStef
Scanning the volume body over the entire trajectory doesn't work??
@ froussel
As explained on page 4, it depends on the size of the part, and therefore on the volume of calculation required from Solidworks to solve the scan.