Beach toys

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carlod3
Posts: 16
Joined: Wed Nov 13, 2013 11:19 am

Beach toys

Postby carlod3 » Mon Jun 08, 2015 12:38 pm

Hi to all.
This is my first post after a long time but I was a passive forum member..

Some days ago I was playing on the beach with my baby girl and I found an interesting product to be made in freecad.

Link to the file:
https://drive.google.com/file/d/0ByBdTd ... sp=sharing


There is no copyright break since I only made it for test freecad capability.
If it is interesting for someone I can write a very long (and boring) post with the workflow, issues, fails and workaroud.

I hope more will come
Attachments
bucket.jpg
bucket.jpg (56.07 KiB) Viewed 3008 times
triplus
Posts: 9475
Joined: Mon Dec 12, 2011 4:45 pm

Re: Beach toys

Postby triplus » Mon Jun 08, 2015 6:16 pm

Looks good.
If it is interesting for someone I can write a very long (and boring) post with the workflow, issues, fails and workaroud.
Sure. Tutorials are always welcomed.
carlod3
Posts: 16
Joined: Wed Nov 13, 2013 11:19 am

Re: Beach toys

Postby carlod3 » Wed Jun 10, 2015 12:17 pm

Premises
I think more than 3 years as passed from my last model posted. The reason is for sure a lot of change in my life. The other is that I haven't find any interesting model to be tested that doesn't need some assembly features.
Now I have find this bucket. It is a new challenge because is not an usual mechanical part.
I am also trying to model the rake part of the beach toys I have, but it is even harder because I have to learn well how to use the loft and sweep features and how to integrate them in my workflow.
My intention is always to obtain the result without design as a power user, so everything is made with the available tools.
Everything is fully parametric and I avoid to use the boolean operations.
I made it with 0.16.4957 on Win7.


Bucket
The workflow I had in mind before to start was:
1. Create one of the six "petal" revolving a profile.
2. Make a polar array of the "petal".
3. Add the details


It was easy to create the petal already with the thickness. I stopped this workflow because I wasn't able to perform the polar array. The reason was that I cannot select the center of the array (the Z axis). The command gives only the possibility to select the axis related to the part itself, or am I wrong?

After some test, this is the workflow I followed:
Cylinder(s) -> draft -> thickness -> upper edge -> handle holes (with a workaround)-> add the handle

Notes
- Since I have started everything at least 5 times. It is good that the sketches remain available if I delete a feature in the tree.
- The sketcher becomes slow really soon adding constrains.
- The sketcher poligon creator make a strange result: I put the poligon center on the origin and the circle on one axis and the result is a poligon edge on the axis (try it..).
- The "merge sketch" doesn't work. It returned to me a wrong sketch and I couldn't remove the unedeed constrains.
- The thickness tool is really slooooow.
- I wasn't able to exclude the edge of the bucket from the thickness operation so I had to apply the thickness before the model complete design.
- Applying the fillet insanely increases the size of the file.
- Applying the fillet on a thin model, if the radius is more the the thickness, the result is wrong. The below image explain the issue. The command must evaluate and avoid this situation.
fillet.jpg
fillet.jpg (5.74 KiB) Viewed 2874 times
- If I undo & redo a feature the "refine shape" is missing.


Handle
I was thinking it was the easiest one but it wasn't.

My first workflow was:
180° revolution -> semisphere terminals -> thickness -> pivots
It failed because It was not able to do the thickness

I tried
180° revolution (with a thickness sketch) -> semisphere terminals (with a thickness sketch) -> pivots
It failed because the revolution to make the semisphere destroyed the entire model.

Finally I had success with this workflow (except for the pivots)
180° revolution -> thickness -> semisphere terminals (with a thickness sketch) -> pivots
At this point I haven't found a workaround for the pivots (the sw doesn't permit to draw a sketch without a planar support).

So I made the sketch of the terminals with the pivot. In this way I had already available one half of the pivot plus a planar surface.
My intention was to make a sketch and a 180° revolution on this face to complete the model but it failed.

At this point I didn't find a solution so I finished the model with the pivots unfinished.
pivot.jpg
pivot.jpg (14.11 KiB) Viewed 2874 times
Notes
- The thickness feature must be improved to work on complex models.
- I had big difficulties with the revolution feature because it fails a lot of times.
- The multitransform feature doesn't work as expected. It is not parametric and applying it two times, it creates two parts. So a boolean operation is needed.

Questions
- I cannot find anymore the option to increase the visual aspect of the model and reduce the "polyline effect" of the arcs and the smoothness of the surface. Where is it?
- How can I select a custom rotation axis?
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quick61
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Re: Beach toys

Postby quick61 » Wed Jun 10, 2015 1:48 pm

Questions
- I cannot find anymore the option to increase the visual aspect of the model and reduce the "polyline effect" of the arcs and the smoothness of the surface. Where is it?
First make sure you loaded the Part Design Workbench, then goto Edit > Preferences... Part Design > Shape view tab and lower the value of the tessellation. I currently have mine set on 0.05% and anywhere around there will be a decent setting.
- How can I select a custom rotation axis?
Insert a construction line where you want the axis of rotation to occur and then select Sketch axis from the Axis pulldown menu. like so -
SketchAxis.png
SketchAxis.png (49.09 KiB) Viewed 2868 times

Edit -
Notes
- The thickness feature must be improved to work on complex models.
Yea, but a lot of times it is asked to do things that just can't be done. Still, it could use some improvment, but i think that's more an OCE thing, not a FreeCAD thing.
- I had big difficulties with the revolution feature because it fails a lot of times.
I have not seen Revolution fail unless it is being ask to perform a function that would result in an invalid geometric object. i think the problems are more user error than tool error.
- The multitransform feature doesn't work as expected. It is not parametric and applying it two times, it creates two parts. So a boolean operation is needed.
Perhaps you can post an example of this in the Help section along with what you are trying to do. This does not sound correct if we are talking about the multitransform feature tool in Part Design.

Mark
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quick61
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Re: Beach toys

Postby quick61 » Wed Jun 10, 2015 2:42 pm

After going back and reading again your issues and problems, I think most all of them can be resolved. If you would like, use the rake model as your working example and post your questions/problems/file in the help section of this forum and myself, along with others will be more than happy to explain how best to use the tools available in FreeCAD and more than likely provide several ways to accomplish whatever tasks you would like to do.

Mark
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carlod3
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Re: Beach toys

Postby carlod3 » Wed Jun 10, 2015 3:02 pm

I reproduced the first fail.



What's wrong?
Attachments
handle_test.FCStd
(17.47 KiB) Downloaded 27 times
revolution_issue.jpg
revolution_issue.jpg (10.32 KiB) Viewed 2855 times
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quick61
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Re: Beach toys

Postby quick61 » Wed Jun 10, 2015 4:00 pm

You have a boatload of geometric errors in the first Revolution. Not quite sure why they were produced, but I ended up redoing everything from scratch as there seemed to be some sort of problem with your first sketch. Here is the model the way I would do it. Notice that i rotated the pins separate from the ends of the handle. This way, I can rotate the pin sketch 360* and the end sketch can then be rotated 180* and everything comes out correct.
Pin.png
Pin.png (36.2 KiB) Viewed 2850 times
Handle_Test(1).fcstd
(60.63 KiB) Downloaded 28 times
Again, these sorts of questions belong in the Help section of the forum, not the showcase. ;)

Mark

OS: Kubuntu 14.04.2 LTS
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Word size of FreeCAD: 64-bit
Version: 0.15.4671 (Git)
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clintonsam75
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Re: Beach toys

Postby clintonsam75 » Fri Jun 12, 2015 2:24 am

That is a fantastic looking bucket! Great tutorial too! Thank you for putting so much passion and hard work into it. You're an excellent contributor. :D
carlod3
Posts: 16
Joined: Wed Nov 13, 2013 11:19 am

Re: Beach toys

Postby carlod3 » Mon Jun 29, 2015 12:32 pm

Here another pieces of my babygirl beach toys set. The watering can!

It is incomplete because I am stuck with no ideas or workarounds to go ahead.

My problems was on the purple part.
Because of the limit of freecad to need a planar surface to draw a sketch, I've started with half of the piece and my intention was to mirror the other half. It cannot be done or I cannot do it..
The other incomplete part is the handle (double T section) because of the fillet on the edge of the sphere. I tried to to make the pocket on the handle before or after the fillet feature, but the final result is wrong with both workflows.
Finally, the thickness feature doesn't work.

The biggest issue IMO is that is often hard to modify the firsts features (e.g. invalid sketch) on the tree, maybe because of the issue with the naming of the faces.
Attachments
watering_can.jpg
watering_can.jpg (61.1 KiB) Viewed 2648 times
watering_can_3.FCStd
(152.3 KiB) Downloaded 34 times
watering_can_2.FCStd
(177.2 KiB) Downloaded 32 times
watering_can_1.FCStd
(9.01 KiB) Downloaded 31 times
watering_can.FCStd
(93.99 KiB) Downloaded 32 times
carlod3
Posts: 16
Joined: Wed Nov 13, 2013 11:19 am

Re: Beach toys

Postby carlod3 » Mon Jun 29, 2015 2:53 pm

Ok, I have found some workaround..

What's wrong now?
- the thickness cannot be more than 0,3mm. (why?)
- because of the above, a not needed thickness is applied also on the handle
- the fillet on the sphere cut is missing

the overall result is quite good now, I think..
Attachments
watering_can_2_2.FCStd
(340.68 KiB) Downloaded 34 times
watering_can_2.jpg
watering_can_2.jpg (61.9 KiB) Viewed 2634 times