Combine, Duplicate & Position

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RussG
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Joined: Wed Apr 27, 2022 11:27 pm

Combine, Duplicate & Position

Post by RussG »

OS: macOS 10.16
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.19.24366 (Git)
Build type: Release
Python version: 3.9.7
Qt version: 5.12.9
Coin version: 4.0.0
OCC version: 7.5.3
Locale: C/Default (C)

I have questions regarding the attached FreeCAD file <Unnamed1>.

The file contains 4 objects within the same Body: First, there is an additive cone. Next a smaller subtractive cone is located within the additive cone thereby creating one object, a hollowed out cone. Together they form a cone with a wall 2.5mm thick, total height 11mm, and a top 1mm thick. The hollowed out section has precise measurements so as to mate with its male counterpart (not included in this file). It took me quite some time to figure out how to do this. When it comes to the method of making the cones, I realize there are different ways of doing the same thing and I tried using sketches and sweeps to make the cones but was not successful. I'm not sure of the best way to do this.

Then, using a sketch I created a padded piece that will act as a connector between the cone and the final piece, the rectangular plate, also made with a sketch and a pad. When finished the project will look like the screenshot attached but the plate will have two cone assemblies and a few holes and partial depth pockets.

Here are my issues: first, I need a second cone/connector assembly and I need to position each assembly precisely 8mm above the bottom edge of the plate. (In the attached file I movied the plate lower by 8mm to accomplish the vertical positioning relationship.) Then I will need to position the cone assemblies, one left of center some number of mm and the other an equal distance right of center.

Is it possible to combine the additive and subtractive cones plus connector into one object so as to then be able to duplicate it? What would be the method? After that, can the assemblies be positioned on the plate with numerical precision using the property editor in the Combo view?

I’ve seen tutorials on duplicating and cloning objects, but invariably they seem to deal with one object, not a combination of subtractive and additive primitives and a sketch that together make one object.

Another problem appears to be that when the cone assembly is exported as an STL file and imported into Prusa Slicer it appears as a solid cone, not one that is hollowed out. It’s no good to me if I can’t print it hollow. Do you think this is a Prusa Slicer thing? A problem making the cone using primitives as opposed to sketches? (I’m not sure how I would do that with sketches.)

Thanks much!
Unamed1.FCStd
(27.89 KiB) Downloaded 12 times
Cone & Plate.png
Cone & Plate.png (125.13 KiB) Viewed 660 times
chrisb
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Re: Combine, Duplicate & Position

Post by chrisb »

For creating the cone I would use a sketch based revolve.

You can clone a complete body. That would clone all additive and subtractive features inside.
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drmacro
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Re: Combine, Duplicate & Position

Post by drmacro »

It is important to understand, there are not 4 objects in the Body.

A Body represents a singlemsolid thatis the accumulation of the feature in the Body. The features can not stand alone as a solitary solid.

The Attachment property of each sketch defines what and how the the Pad/Extrusion/etc. feature Is in relationship to it's predecessor. The last feature, called the tip,is the current state of the accumulation.
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NewJoker
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Re: Combine, Duplicate & Position

Post by NewJoker »

Use two separate Body containers - one for the conical shape and one for the plate. Then you will be able to easily mirror, copy or otherwise move the conical objects without having to apply these operations to the plate as well.

As you can see, mirroring/copying can be done for objects created using multiple operations.

Unamed1_fixed.FCStd
(32.95 KiB) Downloaded 9 times
RussG
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Re: Combine, Duplicate & Position

Post by RussG »

chrisb wrote: Sun Jun 26, 2022 11:27 pm For creating the cone I would use a sketch based revolve.

You can clone a complete body. That would clone all additive and subtractive features inside.
I couldn't figure out how to do that at first, but at your prompting I tried again and succeeded. Something like the attached sketch. I just have to enter the dimensions.

Thanks.
Cone Sketch.png
Cone Sketch.png (34.32 KiB) Viewed 593 times
RussG
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Re: Combine, Duplicate & Position

Post by RussG »

NewJoker wrote: Sun Jun 26, 2022 11:49 pm Use two separate Body containers - one for the conical shape and one for the plate. Then you will be able to easily mirror, copy or otherwise move the conical objects without having to apply these operations to the plate as well.

As you can see, mirroring/copying can be done for objects created using multiple operations.


Unamed1_fixed.FCStd
Based on another comment in another thread I was operating under the belief that all objects that are intended to be manufactured as one part should be modeled within a single body. That's why I placed the components for the cone as well as the plate in the same body. Perhaps I misunderstood or became confused about what I read previously. Now I find myself unclear as to when things should be modeled within the same body and when they should be placed in separate bodies. What s the right way to think about this?
Bance
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Re: Combine, Duplicate & Position

Post by Bance »

RussG wrote: Mon Jun 27, 2022 1:38 amthe belief that all objects that are intended to be manufactured as one part should be modeled within a single body.
This is correct. There is no need for separate bodies.
Here is a file using the techniques described above.
cones.png
cones.png (62.25 KiB) Viewed 522 times
The cones can be re-positioned by changing the attachment offset of the respective sketches. Be aware that only a single solid is allowed, so when moving the pad001 sketch(sketch001) the cone will temporarily disappear. It will re-appear when the cone sketch is also moved. You can select both sketches at once and change their offset together. ;)

(Changing attachment offset position Z will move towards/away from the centre, and position Y up/down. Remember LCS.)
Attachments
mirrorCones.FCStd
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Bance
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Re: Combine, Duplicate & Position

Post by Bance »

To clarify some of what has been said, in Part Design WorkBench (PD WB) the body is a single contiguous solid.

However some the tools work on the features therein, so a mirror(Transform) operation does not mirror the whole solid only the selected features (If all features are selected then all will be actioned.) This allows a flexible workflow, symmetry can be harnessed to allow simple sketches and thus easily maintained models.

FC is a complex organically formed and sophisticated piece of software, It can be utilised in any number of ways to achieve the desired goal. There is NO ONE way of making models.
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NewJoker
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Re: Combine, Duplicate & Position

Post by NewJoker »

RussG wrote: Mon Jun 27, 2022 1:38 am Based on another comment in another thread I was operating under the belief that all objects that are intended to be manufactured as one part should be modeled within a single body.
Theoretically yes but there’s one large limitation in FreeCAD that often makes it necessary to use multiple Body containers even for individual parts - the object has to be continuous. So you can’t make for example two or more pads from separated sketches within the same Body. You have to create separate Body containers for them. And there are also cases when you need more flexibility (e.g. possibility to freely move pieces of a part with respect to each other, as could happen here) so another Body container can be useful.
Bance
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Re: Combine, Duplicate & Position

Post by Bance »

NewJoker wrote: Mon Jun 27, 2022 7:22 amSo you can’t make for example two or more pads from separated sketches within the same Body.
Can you explain this a little more?
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