Best way to build complex part

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chris s
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Joined: Mon Mar 06, 2017 1:23 pm

Best way to build complex part

Postby chris s » Thu Jan 11, 2018 1:07 pm

I have been using FreeCad for about a year so am a newbie. Having terrific fun and have built some stuff that is already printed and working.

But I am confused as to which approach to take when building a complex part. For example, I just tried to build a twin trumpet ram pipe for a car inlet manifold. The ports are rectangular, and have fillets at the corners. So I sketched the profile and swept it using the filleted rectangle as the sweep path. That worked fine for one port, but when selecting an identically shaped port for the second ram pipe it produced a crazy sweep object.

After several attempts I eventually managed to get the second port swept but it took a lot of messing around, and I didnt learn what the problem was. Now the next problem. I wanted to make a flange for the base that covers both ports. I sketched that, but could not pad it without attaching it to a surface - why is that? Surely I should be able to pad any sketch on its own? After more messing around I managed to pad it, but then the pad closed off the ports in the ram pipes, so I then could not figure how to proceed and gave up for now.

I get the impression that it doesnt like the complexity or am I on the wrong tack here? Should I be making the parts in separate designs then merging them all?
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Willem
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Re: Best way to build complex part

Postby Willem » Thu Jan 11, 2018 1:55 pm

hi Chris, as I read your post I do not think the things you want to do are too complex for Freecad. It is just you do not know Freecad very well. Please post your system info and your Freecad file as asked in the forum rules https://forum.freecadweb.org/viewtopic.php?f=3&t=2264.
chrisb
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Re: Best way to build complex part

Postby chrisb » Thu Jan 11, 2018 1:57 pm

You should tell us which version you use and perhaps you can upload your file. Next time don't hesitate too long before asking here.
chris s
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Re: Best way to build complex part

Postby chris s » Thu Jan 11, 2018 2:46 pm

Thanks for the encouragement. Here is the FCStd file. V 0.16. Rev 6706.

Sorry it looks a mess but that's just as I left it!
Attachments
Twin ram.FCStd
(103.86 KiB) Downloaded 12 times
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meme2704
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Re: Best way to build complex part

Postby meme2704 » Thu Jan 11, 2018 3:55 pm

Hi chris s
1st your version is not the last, the last is 6712
there is plenty of duplicate or triple in your drawing, and erases what is useless.
draw only 1 raw, on its 1/2 base trace the flange with its square hole and its round hole for fixation (if necessary), do the extrusion, and make 1 copy mirror
Attachments
pipe.FCStd
(124.26 KiB) Downloaded 8 times
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ppemawm
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Re: Best way to build complex part

Postby ppemawm » Thu Jan 11, 2018 4:50 pm

The problem you are having with the ports is that the model is "forked" at Pad002. In PartDesign make sure that only the last feature is visible when attaching a sketch. Search the forum and you will see that it is a typical error.
chris s wrote:
Thu Jan 11, 2018 1:07 pm
Should I be making the parts in separate designs then merging them all?
In this case it is probably the best approach if using V0.16.

I would have started with the flange:
1. PartDesign/Pad the flange
2. PartDesign/Pocket one port
3. PartDesign/Mirror the other port to complete the flange
4. Part/Sweep one of the ram pipes by multi-selecting top edges of the ports as the path.
5. Part/Mirror the ram pipe across the YZ plane
6. Part/Union (Fusion) the two pipes
7. If you want a single part then Part/Union the Flange with the Fusion of the pipes.
8. Clean up the faces with OpenSCAD/Refine a Copy of the Shape to delete unnecessary coplanar edges.

Picture1.jpg
Picture1.jpg (58.99 KiB) Viewed 376 times
twin_ram2.FCStd
(346.54 KiB) Downloaded 6 times
OS: Windows 10
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.16.6712 (Git)
Build type: Release
Branch: releases/FreeCAD-0-16
Hash: da2d364457257a7a8c6fb2137cea12c45becd71a
Python version: 2.7.8
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 6.8.0.oce-0.17
"It is a poor workman who blames his tools..." ;)
chris s
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Joined: Mon Mar 06, 2017 1:23 pm

Re: Best way to build complex part

Postby chris s » Thu Jan 11, 2018 5:14 pm

Great thanks, I needed that clarity of thinking. Not used mirror before so will add that to my experience.

Just one more thing I have problems with is editing. For example how would be best to change the length of the flange?
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ppemawm
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Re: Best way to build complex part

Postby ppemawm » Thu Jan 11, 2018 8:52 pm

chris s wrote:
Thu Jan 11, 2018 5:14 pm
how would be best to change the length of the flange?
Minor changes can be done in Sketch009, see the following example where the flange has been lengthened by 5mm:

Picture1.jpg
Picture1.jpg (77.58 KiB) Viewed 336 times

Larger changes will likely fail due to "topological naming" issues which you can learn about by searching the Forum. If you want to have a truly parametric model then you will have to use expressions https://www.freecadweb.org/wiki/Expressions with or without a Spreadsheet.
"It is a poor workman who blames his tools..." ;)
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NormandC
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Re: Best way to build complex part

Postby NormandC » Fri Jan 12, 2018 3:35 am

ppemawm wrote:
Thu Jan 11, 2018 8:52 pm
If you want to have a truly parametric model then you will have to use expressions https://www.freecadweb.org/wiki/Expressions with or without a Spreadsheet.
A tip when linking to the wiki: if you know the page name (here, "Expressions"), just type it, select it and click on the "wiki" button to add wiki tags.

In your "Post a reply" window, it will look like this:

Code: Select all

[wiki]Expressions[/wiki]
Which will render as Expressions.