V0.18 Challenge--Clerget 9B Aero Engine--UPDATE #6
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- microelly2
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Re: V0.18 Challenge--Clerget 9B Aero Engine--Work in Process
Wow, very amazing story and impressive pictures
I'm interested how the performance changes when you add all these heavy details.
Where are the limits for comfortable realtime design
Where are the areas to speed up with simplified proxies for details during design process ?
I need some information about the complexity of the model - how many faces of which kind and so on, than I can create randomiced testobjects of the same complexity without any copyrights to see where the bottleneck is and how to get beter performance.
I think I will send you a diagnose script to get more information.
May you publish the dependency graph of your model? A svg file is enough, I can explore it as a first step.
I'm interested how the performance changes when you add all these heavy details.
Where are the limits for comfortable realtime design
Where are the areas to speed up with simplified proxies for details during design process ?
I need some information about the complexity of the model - how many faces of which kind and so on, than I can create randomiced testobjects of the same complexity without any copyrights to see where the bottleneck is and how to get beter performance.
I think I will send you a diagnose script to get more information.
May you publish the dependency graph of your model? A svg file is enough, I can explore it as a first step.
Re: V0.18 Challenge--Clerget 9B Aero Engine--Work in Process
There is no significant slow down in the graphics even though there are a large number of Draft>Arrays, but I do keep most of the model turned off when modelling. I organize the tree with this in mind so that Part sub-assemblies are easy to toggle visible/invisible.microelly2 wrote: ↑Tue Jul 03, 2018 10:03 pm I'm interested how the performance changes when you add all these heavy details.
Where are the limits for comfortable realtime design
Where are the areas to speed up with simplified proxies for details during design process ?
One big slowdown, however, is when it autosaves every 30 minutes which takes about a minute or so but it is enough to break your rhythm. It would be nice if it could do an incremental save.
I have run into this problem before with these larger engine models so there must be a limit somewhere in Graphviz.microelly2 wrote: ↑Tue Jul 03, 2018 10:03 pm May you publish the dependency graph of your model? A svg file is enough, I can explore it as a first step.
"It is a poor workman who blames his tools..."
Re: V0.18 Challenge--Clerget 9B Aero Engine--UPDATE
Yeah. That is the missing part we were talking about in other threads. What you really need now is a good and robust assembly solver and a good organizational strategy. It's doable like you do it now. As you are working on it alone and have the needed skills and a good overview. But it's just like with sketches. Usually you don't want to make sketches too big and complex. And trying to create a "part" of the complexity of the engine is basically doing the same thing. Too big and complex. Simple sketch -> Simple Part -> in the future Assembly of parts. That is the GUI feature you are currently missing and that will likely make your job a bit easier.ppemawm wrote: ↑Tue Jul 03, 2018 9:29 pm A nice GUI feature would be the ability to edit the Attachment while the sketch is open because with this method of modelling multiple bodies you not only have to keep track of dimensions in the sketch but also the offset and revolve angle in the attachment panel. It would also be nice if when starting a new sketch and selecting an origin plane that you also could complete the attachment properties in the same panel. It gets to be a bit annoying to switch back and forth with map mode/attachment and sketcher, especially with a project of this magnitude...103 bodies, 371 sketches, 89 Mb and I am only about 1/3 complete.
Sure. Sometimes that makes sense but in general thanks but no thanks. Too limiting if you know what you are doing.Have been experimenting with attaching sketches ONLY to body origin planes ... External references are absolutely avoided wherever possible ...
If you Pad faces directly and use ShapeBinder and things like that. That is just like attaching sketches to faces and using external reference tool in sketcher. That is when it comes to possible changing topology issues. All this features are prone to the same possible changing topology related issues.However, so far, this has worked out OK and the model is quite resilient to geometry changes except for chamfers and fillets, of course.
Hopefully Draft > Link Arrays will further improve the situation. That is once Links effort gets upstreamed.There is no significant slow down in the graphics even though there are a large number of Draft>Arrays, but I do keep most of the model turned off when modelling. I organize the tree with this in mind so that Part sub-assemblies are easy to toggle visible/invisible.
P.S. But said that we have to work with what we got and you are doing just fine.
Re: V0.18 Challenge--Clerget 9B Aero Engine--UPDATE #2
The parts for the cambox components and valve train have now been completed but not properly aligned. The cams, pushrod assemblies, rockers, and valves will all have to be manually aligned according to the timing diagrams at some point. I anticipate that this will be a tedious process since I am not using any Assembly workbench for this project.
I have been experimenting with copying sketches in lieu of master sketches and external geometry links. You start with the first sketch as simple as possible for the first feature and then copy, toggle construction mode, and add the new geometry. The copied sketch can also be used in a new body. E.g. if you have a sketch to pocket a hole for a dowell then copy the sketch and pad it in a new body to create the dowell in the exact location. While this is quite efficient and helps to build a remarkably robust model, it does has some disadvantages. If you have to make a change in the sketch geometry or attachment offset then you have to change all the copies as well since they are not linked. I have not decided if this is a better method but have been burned too many times using shapebinders and external links when it comes to making changes that effect the number of edges and vertices, especially in complicated bodies with many features.
The parts added with this update are shown in the following pictures with a few comments:
. . . . .
The file has grown to 116 Mb and sketch count is at 573. Even so, the overall performance is quite satisfactory except when opening the file or during autosave which takes several minutes.
The next parts to be tackled are the reciprocating components (connecting rods and pistons) and then the accessories such as the air/oil pumps and the magnetoes. These latter parts will be a real challenge due to their complexities and highly featured lightweight housings. Stay tuned for next month's update.
OS: Windows 10
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.18.13983 (Git)
Build type: Release
Branch: master
Hash: 8f1c6f77c090ae7d9c2bfd4f18811083b01a3eb2
Python version: 2.7.14
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 7.2.0
Locale: English/UnitedStates (en_US)
I have been experimenting with copying sketches in lieu of master sketches and external geometry links. You start with the first sketch as simple as possible for the first feature and then copy, toggle construction mode, and add the new geometry. The copied sketch can also be used in a new body. E.g. if you have a sketch to pocket a hole for a dowell then copy the sketch and pad it in a new body to create the dowell in the exact location. While this is quite efficient and helps to build a remarkably robust model, it does has some disadvantages. If you have to make a change in the sketch geometry or attachment offset then you have to change all the copies as well since they are not linked. I have not decided if this is a better method but have been burned too many times using shapebinders and external links when it comes to making changes that effect the number of edges and vertices, especially in complicated bodies with many features.
The parts added with this update are shown in the following pictures with a few comments:
. . . . .
The file has grown to 116 Mb and sketch count is at 573. Even so, the overall performance is quite satisfactory except when opening the file or during autosave which takes several minutes.
The next parts to be tackled are the reciprocating components (connecting rods and pistons) and then the accessories such as the air/oil pumps and the magnetoes. These latter parts will be a real challenge due to their complexities and highly featured lightweight housings. Stay tuned for next month's update.
OS: Windows 10
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.18.13983 (Git)
Build type: Release
Branch: master
Hash: 8f1c6f77c090ae7d9c2bfd4f18811083b01a3eb2
Python version: 2.7.14
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 7.2.0
Locale: English/UnitedStates (en_US)
"It is a poor workman who blames his tools..."
Re: V0.18 Challenge--Clerget 9B Aero Engine--UPDATE #2
Man, you are one dedicated and patient man. Amazing work!
You are right that a sweep with more than one sweep path would really be useful (have you checked out Chris_G's Curves wb? I believe it has one, but I haven't tried it). Nonetheless, I was able to get the 10mm radius in the sweep shape by adding an intermediary sketch.
I first created a master sketch to determine where to position the cross-sections, on which I also based my datum planes for the cross-section sketches.
Then I first created a simple 2-section AdditiveLoft:
And I added an AdditivePipe for the smaller end, using Sketch's short R10mm arc at the forefront as path.
Then I added the cylinders and added fillets.
Note that for the centre cylinder, I had to go back to the first Sketch and remove the tangency between the bottom slanted line and the circle, or the fillet would fail. Oddly enough, tangency wasn't problematic on the 3 other junctures.
Of course I had to leave PartDesign to make a Part Mirror and a Part Fuse. I sure hope that at some point in the future, somebody implements the "PartDesign Mirror Body" feature I asked for last year. (issue #2863)
I didn't bother modelling the complete part, and the dimensions were really hard to read in the screenshot.
Hope this helps...
Norm
P.S. Adding an OpenSCAD Refine Shape feature removes the split edges on the cylinders and makes the part look nicer. My FCStd file doesn't include it to reduce file size.
If you look closely at P. Jensen's screenshots of his 3D model, you can see that there is a parting line along the XY plane. I'm pretty sure he only modelled the top half then mirrored it. I think that's how he could do these fillets without need for "fillet stops".ppemawm wrote: ↑Tue Jul 24, 2018 4:49 pm Of all the parts, the rockers were the most challenging and frustrating. I simply was not able to create a model according to the drawing. The problems were the 10 mm radius at the juncture of the valve end of the rocker, the elliptical cross section, and all the fillets.
The arrow points to the trouble area. It seems the only way to duplicate this properly as shown in Jansen's drawing and his original model of the actual part is to use a sweep with two sweep paths, of course, something FreeCAD does not have. The best I could do was a 5 mm fillet radius all around. Looks good but not perfect.
I also tried a 10 mm Part>Variable fillet but it will not exactly duplicate the 3 mm fillet radius shown on drawing.
Perhaps someone has a suggestion for a different approach?
You are right that a sweep with more than one sweep path would really be useful (have you checked out Chris_G's Curves wb? I believe it has one, but I haven't tried it). Nonetheless, I was able to get the 10mm radius in the sweep shape by adding an intermediary sketch.
I first created a master sketch to determine where to position the cross-sections, on which I also based my datum planes for the cross-section sketches.
Then I first created a simple 2-section AdditiveLoft:
And I added an AdditivePipe for the smaller end, using Sketch's short R10mm arc at the forefront as path.
Then I added the cylinders and added fillets.
Note that for the centre cylinder, I had to go back to the first Sketch and remove the tangency between the bottom slanted line and the circle, or the fillet would fail. Oddly enough, tangency wasn't problematic on the 3 other junctures.
Of course I had to leave PartDesign to make a Part Mirror and a Part Fuse. I sure hope that at some point in the future, somebody implements the "PartDesign Mirror Body" feature I asked for last year. (issue #2863)
I didn't bother modelling the complete part, and the dimensions were really hard to read in the screenshot.
Hope this helps...
Norm
P.S. Adding an OpenSCAD Refine Shape feature removes the split edges on the cylinders and makes the part look nicer. My FCStd file doesn't include it to reduce file size.
- Attachments
-
- ppemawm_exhaust_rocking_lever_test_nc1.fcstd
- (837.28 KiB) Downloaded 83 times
Re: V0.18 Challenge--Clerget 9B Aero Engine--UPDATE #2
Thanks NormandC.
I swear I tried everything but that. Tunnel vision I guess.
Anyway, now you have a body in my engine model. A simple and elegant PartDesign solution.
EDIT: Note that you can make a PartDesign>Mirrored feature by stacking the features in the same order
as created in the mirrored parameters list then add the fillets.
One again you have proven why you are the MAN.
"It is a poor workman who blames his tools..."
Re: V0.18 Challenge--Clerget 9B Aero Engine--UPDATE #2
Aw man, no, you are the man.
Unfortunately, this sweep is not perfect. The rear is not perfectly straight. Just to find out, I placed a large cube tangent to both cylinders and made a Part Cut.
You can see where the sweep was exceeding the line, the cut generated two planar faces (in grey).
- Attachments
-
- FC_ppemawm_exhaust_lever_05.png (43.39 KiB) Viewed 2538 times
Re: V0.18 Challenge--Clerget 9B Aero Engine--UPDATE #2
It's not working for me, creating PD fillets after a PD Mirrored feature fails.
I think I'll try another approach than the AdditiveLoft + AdditivePipe.
Re: V0.18 Challenge--Clerget 9B Aero Engine--UPDATE #2
This is really great stuff. Most impressive was the hairneedle spring to me. Did you use a helix for the middle part of it?
A Sketcher Lecture with in-depth information is available in English, auf Deutsch, en français, en español.
Re: V0.18 Challenge--Clerget 9B Aero Engine--UPDATE #2
Yes.
The drawing shows two, one larger half outer helix, and a smaller inner helix on different centerlines. The wrap of the inner helix was adjusted to align the horizontal pad with the valve cap, the horizontal pad was trimmed at the valve cap centerline, and finally, a quarter revolve around the cap finished it off. Not as tricky as it may appear.
"It is a poor workman who blames his tools..."