polar pattern around standard axis?

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ShurikMur
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Re: polar pattern around standard axis?

Post by ShurikMur »

I trying to accomplish some tasks that feels beyond of functionality of part design WB mode,
bejant wrote:If you can show us what you're trying to model maybe we can offer better help to get you started.
I trying to make a propeller with a several blades and a hub/spinner.
Each blade must have exact foil (in fact two: one at the root and another on the tip), and the tool to create 3D object with a smooth transition from one sketch to another can be fount in complete WB, wrong, part WB (what the difference with part design WB? Also unclear to me).

Watched some tutorials on youtube about making propellers in a FC, but not all clear for me and they are also using some workarounds...
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blade01.gif
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quick61
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Re: polar pattern around standard axis?

Post by quick61 »

(what the difference with part design WB? Also unclear to me)
This is probably the source of most of your confusion.

Part Design Workbench is intended to construct a single complex solid for a series of simple features. When you start a project in Part Design, you always begin with an additive feature such as a Pad or Revolve, never a subtractive feature like Pocket of Grove. Once that first Feature is created, you then apply to that single solid, additional features, which can then be either additive or subtractive, but are always features of that same base solid. This is considered to be linear construction.

In the Part Workbench, you have tools to make solids from shapes and then to make new solids through boolean operations between 2 or more solids.

Lets take a simple example. A basic cube with a hole in the center. First let's construct that in Part Design.

1 - Make a Square sketch 10 mm each side and Pad that Sketch 10 mm.
Shot1.png
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2 - Now click on that Cubes top surface and create a new Sketch and make a 2 mm radius Circle in the center and Pocket it Through all. That pocket is now the second feature of the single solid.
Shot2.png
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Now start a new document and switch to the Part Workbench.

1 - Click on the default Cube and then the default Cylinder. Notice that you now have 2 separate solids in your new document.
Shot3.png
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2 - Using Edit > Placement ... change both the X and Y Translation values to 5 mm. This will put the Cylinder in the center of the Cube. Now Select Cube, then holding on the [Ctrl] key Click on Cylinder in the tree view, (in that order), and then select Cut from the toolbar.
Shot4.png
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3 - Now select Cut from the tree and go to Edit > Placement ... and change both the X and Y Translation values to 30 and click OK. now expand Cut in the tree view and make both Cube and Cylinder visible. What you have now are 3 separate solids. Cube, Cylinder and Cut which is parametrically linked to the difference between the first two solids but is in fact separate 3rd solid.
Shot5.png
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This method of construction is called CSG, or Constructive Solid Geometry. While both methods produce the same looking part, they in fact accomplish this in very different ways.

Constructing something like a propeller is NOT a task for someone new to FreeCAD, or any parametric CAD for that matter. You really need to have a grasp of the basics first and that is something that is not learned overnight. It can take weeks, if not months.

To pick up on another note. FreeCAD is a Solid Modeler and has the capability of converting solids into meshes, usually for export or FEM analysis. Within FreeCAD, you either import a mesh or you intentionally created one. They just don't pop up out of nowhere and when you have one imported or intentionally created, they have a unique icon in the tree view and a different color (by default) in the 3D view.

Mesh icon - Image which looks completly different from Solid or Shape icons, so it is very easy to tell the difference, once one learns the basics.

As it has been said before, CAD is hard. Once that fact is accepted and one makes the decision to learn, you'll quickly find out that it is not impossible and maybe not all that hard as it first appeared. ;)

Mark
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ShurikMur
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Re: polar pattern around standard axis?

Post by ShurikMur »

quick61 wrote: As it has been said before, CAD is hard. Once that fact is a... ;)
...
Mark
That's not true, just because CAD, like any other software, is made for people :)

Back to business:

Many solids or one with features - does not explain why I can't copy some object, a separate solid, in some pattern. Can you just tell me how to duplicate a blade several times and assign by a raw numbers angle of rotation among specified axis? (i know how to copy, but can't properly rotate them)

BTW, in some other CADs and 3D modelling software - if you assign some objects into a single group - you always can manipulate this group as a single 3D object with the same set of tools. Nobody cares if it is a single object or a result of fusing many objects together. :)
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quick61
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Re: polar pattern around standard axis?

Post by quick61 »

ShurikMur wrote:
quick61 wrote: As it has been said before, CAD is hard. Once that fact is a... ;)
...
Mark
That's not true, just because CAD, like any other software, is made for people :)

Back to business:

Many solids or one with features - does not explain why I can't copy some object, a separate solid, in some pattern. Can you just tell me how to duplicate a blade several times and assign by a raw numbers angle of rotation among specified axis? (i know how to copy, but can't properly rotate them)

BTW, in some other CADs and 3D modelling software - if you assign some objects into a single group - you always can manipulate this group as a single 3D object with the same set of tools. Nobody cares if it is a single object or a result of fusing many objects together. :)
You will probably want to use Draft Array. I know, I've often thought there should be a Part Array, but no one thinks it important enough to code into the Part Workbench when Draft Array works so well. Select your part, and apply Draft array to it and use the array type polar and give it the number polar you wish. You can also Draft Clone your part and position them as you see fit. Both Array and Clone will have their children linked to the original.

Here is an example using Draft Array and a simple propeller blade distributed in 3 positions around a hub. I created one of the blades with a Loft between 2 airfoils, arad20 at root, arad10 at tip, then positioned the loft with Placement, applied Array and fused everything together.

Link to file - https://www.dropbox.com/s/aesl1fled0lbx ... fcstd?dl=0
3Prop.png
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Edit - here is one with a simpler made up airfoil that is a much smaller file, same principle, though the loft has a few BOPAlgo GeomAbs_C0 errors in it, which were carried through to the Draft Aray. :( But it does present the technique used in modeling such things.
3Prop1.fcstd
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3Prop1.png
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Mark

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triplus
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Re: polar pattern around standard axis?

Post by triplus »

ShurikMur wrote:(big post, related to UX and a workflow of a freeCAD in general)
jmaustpc wrote:Its rather complex, there are all sorts of complications that arise not least of which is compatibility....if it was easy it would have been introduced years ago...
The more I digging into FC, the more it feels broken to me. :?

The main issue - the editing options in general (if look at all of them in all editing modes) are very restricted and specifically dedicated to some exact objects. Some works with features, some - with solids, some - with a 2D sketches. It is VERY unclear to user: one may understand the major difference between 2D sketch and 3D object, but other than that - all 2D editing tools should work with all 2D objects, and all 3D tools - with all 3D objects.

For example, for almost an hour fighting with FC, trying to rotate 3D object, created by using the loft utility from 2 sketches (It's a solid? body? feature? or maybe mesh? Not obvious at all! :o For the user it is just some solid 3-D object, point.). Polar pattern doesn't work, some rotate function (found in "Complete" editing mode) says it can rotate objects, but is somehow restricted to some plane (how to choose that plane?...) and not friendly in general, "transform" option does not allow to perform exact transformations (in mm and degrees) and, even worse, does not supports undo!!! Rotated object can't be restored to last position, if you occasionally moved or turned it... How simplier and better could it be, if there was universal 3D-manipulating tools for all 3D objects!

The pop-up description of tools are also unclear and too short.

IMHO, for the clear UX and maximum usability, all compatibility-related features should be separated into another "layer" of application: through exports, conversions e.t.c.
I still believe in a freeCAD, it is great to have such a promising alternative to paid products, but the workflow kills me :shock:
If you learned all that in one hour i am sure you will get basic understanding of the concepts fast enough. ;)
ShurikMur
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Re: polar pattern around standard axis?

Post by ShurikMur »

quick61 wrote:You will probably want to use Draft Array...
Thanks for the detailed answer will check this out!
Torsten
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Re: polar pattern around standard axis?

Post by Torsten »

First of all: thanks a lot for that great 3D-Modelling software and my respect to all developers working on it. You are doing a really great job!
Users claiming features here should have in mind, that we have a software for free, where others pay thousands of Euros for... so, what do you want for nothing? ;)

I was struggling with the same issue, unfortunately the "Select Reference..." feature doesn´t work at all - not even the solution posted here with creating a dummy solid and selecting an edge as reference did it. No selection was possible.

The Draft Array solved it. For others, here a little step-by-step manual for the workaround. If you find it a bit unprofessional, please bare with me, I use FreeCAD since only two weeks now... :oops:
The shown screenshots are from a test object to learn the basics, since I didn´t want to shoot my real project.

1. The task was, to have 15 pinions on each teeth of the part. First, a circular scetch was designed and the extruded to a pad:
Task.PNG
Task.PNG (190.68 KiB) Viewed 2258 times
2. Change to the Draft workbench, select the pad and klick on the Array button. In the example, 15 pads are necessary around 360° (15x 24°). Setup you parameters (Polar selection is important!) and - you´re done!
array.PNG
array.PNG (299.94 KiB) Viewed 2258 times
3. Other increments and/or fractions of the circle are possible as well, but you have to calculate the total angle manually then:
array_fraction.PNG
array_fraction.PNG (306.15 KiB) Viewed 2258 times
Hope, it helps others fighting with that!

Best regards

Torsten

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Last edited by Torsten on Tue Feb 16, 2016 6:11 pm, edited 5 times in total.
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jmaustpc
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Re: polar pattern around standard axis?

Post by jmaustpc »

Your first post, welcome to FreeCAD. :)
Torsten wrote:unfortunately the "Select Reference..." feature doesn´t work at all - not even the solution posted here with creating a dummy solid and selecting an edge as reference did it. No selection was possible.
Please always post your Help menu ...about FreeCAD information, its very frustrating having to continuously ask people for this. How to do so is explained in the first topic at the top of the Help forum

Important:readbeforeaskingforhelp

The feature you are talking about works fine, PartDesign Polar Pattern Feature, here is a simple example file
polarpattern_select_reference.fcstd
(19.63 KiB) Downloaded 60 times
I would guess from your screen shots that the problem for you was that you might not have understood that you have to select an edge of the solid that the sketch is mapped to. You map a sketch by first selecting the desired face then clicking on new sketch, or it is possible to create a sketch first and then click on "map sketch to face".

Also there is a new version of PartDesign in a development branch that will hopefully be merged soon after 0.16 is released. It has many new features , including some that would have helped in similar circumstance to yours. :)


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Torsten
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Re: polar pattern around standard axis?

Post by Torsten »

Thanks for the welcome and best regards half around the world!
I´ve edited my post and added the Version Infos, you´re right, that might be helpfull sometimes.

I understood, that the scetch has to be related to the solid where the later turning edge belongs to. My problem was, that the circular scetch could not be related to the outer diameter of the part (since it is not a flat surface) and relating the scetch to a "dummy" solid always moved the scetch in the wrong position... for shure a beginners problem, I simply didn´t find the right way.

FreeCAD is very powerfull, but sometimes a bit hard to get in. It´s getting better every day, but I wouldn´t say that I really have a clue after the two weeks now.

I will try your sample project tomorrow, thanks a lot for your help!
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jmaustpc
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Re: polar pattern around standard axis?

Post by jmaustpc »

Torsten wrote:My problem was, that the circular scetch could not be related to the outer diameter of the part (since it is not a flat surface)
That's why I knew your sketch was not mapped to the face. :) The work around of adding temporary features to provide you a face to mount the sketch to does work, and would work in your example but it only ever was a "work around" of current limitation. The proper method is going to be in the new PartDesign workbench that is hopefully coming soon.

Please remove your version data from you signature file, other wise when you eventually update all your old posts will show the wrong data. This is requested in big, huge, red text in the first topic at the top of the Help forum....

IMPORTANT: Please read first before asking for help

Your FreeCAD version is now looking almost obsolete, there are over 1500 bug fix and new feature commits in 0.16 after 0.15. I recommend you try out a 0.16 snapshot or from the "daily" PPA etc.
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