Without curve guides the removal of tendril material ...
That's why I use the guide curve:
I don't know how you generate the trajectory curve, have you tried to draw it flat and then make a winding? This would guarantee the continuity and tangency of the different segments.
Then use this path for volume scanning
Good evening @LeStef,
A relatively simple proposal, which seems to work. The steps:
- a cylindrical body on which two propellers are wound 180° apart;
- a plane tangent to the cylinder to construct the connection sketch consisting of two arcs and a segment. Tangency constraints with the propellers ensure continuity. The sketch is then wound on the cylinder ;
- the same principle in the lower part for the entrance and exit of the groove;
- a 3D sketch that groups together in the form of a single 3D spline the two helices, the connection contour and the wound inputs/outputs. Use of the "Convert entities" and "Adjust spline" functions, always for the purpose of continuity;
- sketch in the basic plane of the cylinder to build the groove profile, and finally, a material removal by scanning.
Visually, the result is correct. Even if the reconstruction is sensitive to changes...
The file is attached (SW 2018).
helice_double.sldprt
2 Likes
Hello m.blt,
The idea is good but the problem is that the scan sketch does not remain tangent to the surface of the cylinder during the scan... it goes awry!
I tried to do the same thing but with a removal of material by a volume, but Solidworks doesn't want to take the 3d spline for the trajectory...
I tried by splitting the work into two steps to relieve Solidworks by starting the sweep at the bend:
The first half works well
The second part, Solidworks loses its way... approximate trajectory in shape and depth...
I'm drying!
OK... So what?
If the trajectory is relatively simple, it works very well. Below is a video that explains the process well.
https://www.youtube.com/watch?v=T2-N_9KRm4s
But with more complex geometry, Solidworks doesn't manage... and throw in the towel!
Which version of SW are you in
Here is a cross-sectional view, the shape is perfect
vue_en_coupe_-_enlevement_gorge_2021-03-05_12_53_07-window.jpg
Version 2020 SP4.
Hello @LeStef,
Indeed, the twisting of the section had escaped me, due to a groove bottom of a circular section, which largely masked the phenomenon.
This mistake suggested a lead for me: I made a first removal-sweep with a circular section, on which the twisting has no effect.
I then used the two edges of this groove to serve as a trajectory and guide curve for a sweep with a rectangular section groove.
This procedure seems to improve the "guidance" of the section and gives a result close to the expected...
Maybe still imperfect, but what is the criterion for validating perfection?
My limit has been reached!
helice_doublev2.sldprt
1 Like
Hello @LeStef
so your main concern if I understand correctly
It's that your profile doesn't follow your 3D sketch correctly since it's not always perpendicular to your wall
So I offer you a tip ;-)
make your complete 3D sketch
on the cylinder having as a section the diameter corresponding to the axis of the radius of your material removal, considering that you are going to do a sweep with a circular section like this even if it twists it won't matter since it's a circle
then you just have to create a surface offset by the minimum on the surface and thicken this said surface to get the right clearance for your heating cable the remaining half diameter + margin ;-)
and that's it
@+;-)
2 Likes
In reply to m.blt,
Indeed, the expected result must be impeccable... The length and complexity of material removal pushes Solidworks to its limits. On a short length it works.On this length (400 mm) Solidworks pedals for 10 to 15mm before giving up.
That's why I'm wondering about the limiting factor... Solidworks ? My machine ? my config ? a little bit of everything...
1 Like
To make your 3D sketch you can also start from a helix , for this you create your helix, create an empty 3D sketch, select your helix and convert it (convert entities.)
Then it's up to you to add your hook at the top while staying tangent. Then you create your body and you subtract it.
Easy to say, a little more complicated to achieve.
And for the record, we have screws made on the same problem and we too it grinds a lot, not 5 minutes but not far.
2 Likes
Good evening
For me, machine time is 10 seconds. SW doesn't muffle by the way, I stole the sponges so he can't throw it away.
The machine keyboard interface is 30 minutes (once you know how to do it).
And I don't do any 3D sketches in the strict sense. (I'm quite close to the technique proposed by @sbadenis at least for the idea of the propeller.
It can be used in CNC directly!
Kind regards
Hello
I tested your gt22 trick , but the thickening crashes...
Indeed your remarks are relevant, and initially I had used the insertion of helical curves, with removal of material by a body.
And for the turn, a rolled up sketch.
It works without crashing, I even have a room with two footprints:
But the junctions between the different parts of the footprint are not clean.
That's why I tried another method to do the full scan at once to avoid the junctions.
I repeat the sweeping exercise with a trajectory and a guide curve on a cylinder 100mm long, Ø 14.9mm, propeller pitch, 12mm turn, two arcs, radius of curvature min 4.5mm.
it works, the result is perfect!
The same thing on a 150mm long cylinder, Solidworks heats up for 7 to 8 minutes and then lets go...
100mm is fine, 150mm is not, and I would like 400mm...
That's why I made this post, soliciting the experiences of users to see if there would not be a hardware explanation, config ... something that escapes me...
Thank you
Hello
Why do you absolutely want to do the forward + 180° turn + return sweep in one go?
There are several paths that lead to rum!
It seems to me that the goal is rather to make the perfect part for CNC machining even if it is not made in a single scan.
There is no difficulty in doing it even in 2m long if necessary.
Kind regards
1 Like
Why all at once?
Because when cutting out the different parts, there are always small defects at the junctions.
So I wanted to go all the way with the idea of making the whole thing in one go.
Hello @LeStef,
Would it be possible to have the 3D of the part as it works (in 100 mm for example)? Without that, I'm afraid that the subject won't go any further.
If it's confidential but can be distributed in the company, you'll easily find me in the internal directory...
M.
Yes and if possible in parasolid
That way, even with a different version, it will be possible to answer you
What is the diameter of your heating cable
@+