Sweep - Deformation of profile

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Lars
Posts: 19
Joined: Sat May 05, 2018 10:39 am

Re: Sweep - Deformation of profile

Postby Lars » Sat Jul 04, 2020 1:33 pm

Dear all,
Thank you for your support and valuable input for resolving this issue of designing a coil consisting of straight parts combined with bends with constant radius. The item is a heat exchanger and the bending machines are are capable of producing items with straight parts or bends with constant radius. In order to produce the coil which has a continuous change of bending radius, we need to convert the design into parts suitable for manufacturing.
The trick that resolved the issue was the WB curves and draft, creating the center line of the item by connecting end points of 3-point arc (macro) with straight lines, followed by a sweep.

The section feature identified by Hammax is far more simple and less time consuming, compared to the solution we used.
Thank you so much for your contribution and assistance!
BR
Lars
Best regards

Lars
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tanderson69
Posts: 1545
Joined: Thu Feb 18, 2010 1:07 am

Re: Sweep - Deformation of profile

Postby tanderson69 » Sun Jul 05, 2020 7:49 pm

hammax wrote:
Wed Jun 17, 2020 3:16 pm
... a really interesting task, to build a helical pipe with a controlled contour - more than cylindrical or conical.
Yes it is. I used DRAWEXE to create a pcurve from the contour surface and used that for the sweep spine. With this, the coil wraps are more evenly spaced along the contour surface.

original:
intersection.png
intersection.png (103.16 KiB) Viewed 686 times

pcurve:
pcurve.png
pcurve.png (145 KiB) Viewed 686 times
Attachments
pedge.brep
(5.77 KiB) Downloaded 12 times
Lars
Posts: 19
Joined: Sat May 05, 2018 10:39 am

Re: Sweep - Deformation of profile

Postby Lars » Tue Aug 18, 2020 7:36 am

Dear all.
Following the successful design of a conical coil as previously discussed, manufacturers of numeric bending machines faces difficulties in achieving a successful import and processing.
Instead, they now suggest a modification of the coil shape design from circular to squared as indicated in the attached file. However, when sweeping the tube profile along the center line designed in the way suggested by you, the sweep fails. It appears that the center line somehow is not properly connected.

I would be very grateful for any suggestions how to overcome this issue?

OS: Windows 10
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.18.4 (GitTag)
Build type: Release
Branch: releases/FreeCAD-0-18
Hash: 980bf9060e28555fecd9e3462f68ca74007b70f8
Python version: 3.6.6
Qt version: 5.6.2
Coin version: 4.0.0a
OCC version: 7.3.0
Locale: English/UnitedKingdom (en_GB)
Attachments
A25 Separator LTHW coil ver01e.jpg
A25 Separator LTHW coil ver01e.jpg (67.21 KiB) Viewed 642 times
A25 Separator LTHW coil ver01ea.FCStd
(60.74 KiB) Downloaded 17 times
Best regards

Lars
chrisb
Posts: 30868
Joined: Tue Mar 17, 2015 9:14 am

Re: Sweep - Deformation of profile

Postby chrisb » Tue Aug 18, 2020 8:04 am

Concerning the loft:
- You should always use point-to-point tangency if applicable. In Sketch-Top the selected constraint should be changed appropriately:
Snip macro screenshot-ad24b3.png
Snip macro screenshot-ad24b3.png (12.7 KiB) Viewed 640 times
- You most probably want to set Closed=false: the last section should not be connected to the first.

However, the final result still looks like some delicious French Mergueze.
Changing the AngularDeflection to a smaller should help; alas, I have set it to 2.5 and now my computer is at 100% since 15 minutes. You may try a bigger value or a faster computer.
You need at least FreeCAD 0.19.23300 to edit my current sketches.
A Sketcher Lecture with in-depth information is available in English, auf Deutsch, en français, en español.
chrisb
Posts: 30868
Joined: Tue Mar 17, 2015 9:14 am

Re: Sweep - Deformation of profile

Postby chrisb » Tue Aug 18, 2020 8:36 am

Killed the process after another half hour.
You need at least FreeCAD 0.19.23300 to edit my current sketches.
A Sketcher Lecture with in-depth information is available in English, auf Deutsch, en français, en español.
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papyblaise
Posts: 2913
Joined: Thu Jun 13, 2019 4:28 pm
Location: France

Re: Sweep - Deformation of profile

Postby papyblaise » Tue Aug 18, 2020 8:36 am

Use Partdesign it's better way to do it
the file is to large : 6.2Mo
Attachments
squared coil.PNG
squared coil.PNG (269.6 KiB) Viewed 631 times
chrisb
Posts: 30868
Joined: Tue Mar 17, 2015 9:14 am

Re: Sweep - Deformation of profile

Postby chrisb » Tue Aug 18, 2020 8:42 am

Is this with the default deviation of 28.5°?
You need at least FreeCAD 0.19.23300 to edit my current sketches.
A Sketcher Lecture with in-depth information is available in English, auf Deutsch, en français, en español.
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Roy_043
Posts: 2398
Joined: Thu Dec 27, 2018 12:28 pm

Re: Sweep - Deformation of profile

Postby Roy_043 » Tue Aug 18, 2020 9:48 am

Would it not be possible to create the squared coil from arcs and straight lines? I suspect that that is the intention of the manufacturer(s). The current path is the intersection of a conical sweep and a helical face. So mathematically quite complex.
Lars
Posts: 19
Joined: Sat May 05, 2018 10:39 am

Re: Sweep - Deformation of profile

Postby Lars » Tue Aug 18, 2020 10:50 am

papyblaise wrote:
Tue Aug 18, 2020 8:36 am
Use Partdesign it's better way to do it
the file is to large : 6.2Mo
I do not follow your suggestion, but would be grateful for clarification of a more suitable way for generating the center line of the coil?
Best
Lars
Best regards

Lars
User avatar
tanderson69
Posts: 1545
Joined: Thu Feb 18, 2010 1:07 am

Re: Sweep - Deformation of profile

Postby tanderson69 » Tue Aug 18, 2020 10:56 pm

I was able to get something using the same process I used before (I didn't use freecad):
Created a periodic bspline from sketch. I think that can be done from Draft and or python.
Swept that along a line using a law curve. That process can be simulated using multiple profiles.
Created a series of pcurves on the swept surface. Not sure if/how this is done in freecad.
Build 3d edges from pcurves and created wire. Not sure if/how this is done in freecad.
Used circle and the wire in a sweep using constant binormal. I think part design can do constant binormal sweep?
Instance and unite.
There are a couple of really loose vertex tolerances and bopcheck has some C0 issues.
spring3.png
spring3.png (139.04 KiB) Viewed 553 times
Attachments
spring3.brep.zip
(914.31 KiB) Downloaded 5 times