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Splitting Solids? - **Solved**

Hello Everyone,

I am working on a practice project and need some guidance. Basically, I am trying to fully model a part, then create layered slices of that part which can be laid out onto sheet-good materials for CNC routing.


Screenshot 2022-01-20 160917.pngScreenshot 2022-01-20 161048.png
Intuitively, I want to create an array of planes spaced one material thickness apart which I would use to split the cone into slices, however this functionality doesn't seems available, to my knowledge, in Alibre v24.
(
Here is an example of fusion360 handling the task if my explanation didn't fully explain the desired result)


Fig1Screenshot 2022-01-20 162408.png Fig2Screenshot 2022-01-20 162451.png Fig3Screenshot 2022-01-20 162518.png
I have attempted using an assembly workspace to create a cone slice through a boolean operation. While successful the process is time consuming requiring the creation of a solid block tool (fig1), a working boolean (fig2), and finally the resulting slice with a boolean between the [working boolean] and [block tool] (fig3).


Screenshot 2022-01-20 164118.pngScreenshot 2022-01-20 164156.png
I have also explored using surfaces to split the cone. While this solution also works it is also quiet time consuming needing, again, a solid block tool to pull a surface from then cutting the cone with that surface. Another issue with this method seems to be it becomes more complicated as multiple slicing operations are needed to cut pieces from the center of the cone.

Screenshot 2022-01-20 170158.pngScreenshot 2022-01-20 170730.png
In this example of a cone, I could also break down the slices into individual parts from the get go, each with its own sketch, and just revolve each part and add them into an assembly for CNC layout purposes. The worry with this method is once the overall part being sliced reaches a certain level of complexity the idea of hand drawing every layer becomes unreasonable.


If anyone has a method that is more practical and faster than the above mentioned I would love to find out your secrets! I have searched the forums for this topic and did manage to find some suggestions, one being to use configurations but I am not sure where to start with that approach. Also I found this article in the Help Files: Slice a Part , but again I'm not sure how to make this work for me.

Thank you for reading my post and giving it your time and thoughts!
All the best, Konrad
 

wsimonton

Senior Member
You can create the Planes, and use the Precise Section Views to Cut the Part (show the Section), and then starting from the Plane of the Section creating the View, use 2D Sketch and Project to Sketch on the surface to create the drawing(s) with one command. I have used that on numerous occasions to create drawings of sections through a Part which is created with numerous curves and splines.
 
You can create the Planes, and use the Precise Section Views to Cut the Part (show the Section), and then starting from the Plane of the Section creating the View, use 2D Sketch and Project to Sketch on the surface to create the drawing(s) with one command. I have used that on numerous occasions to create drawings of sections through a Part which is created with numerous curves and splines.
Hello wsimonton,
I tried your method, or at least attempted it.
Screenshot 2022-01-20 234629.pngScreenshot 2022-01-20 234613.pngScreenshot 2022-01-20 234645.png
When I use the precise section view it seems like I can only divide the part from one side/one division. The images above used planes spaced 3/4" apart, the first slice is correct but the subsequent slices include too much of the original cone.

Screenshot 2022-01-21 000632.pngScreenshot 2022-01-21 000704.png
Is it possible to create a slice like in this example using your method?

Also, are you able to clarify your use of the Project to Sketch tool? From that I gathered from your reply you would be using the sketch generated from the precise section view as the figure for the CNC to cut out. If this is the case wouldn't the cone become a stack of reducing cylinders instead of tapered cone sections?

Something like this:
Screenshot 2022-01-21 002353.png

Thanks for your response by the way!
 

HaroldL

Alibre Super User
If you start with a basic sketch constructed of Reference Geometry:
refBaseSketch.png

Then trace each layer in turn with Sketch Figures, Revolve and SAVE AS:
OutlineEachLayer.png

After each SAVE AS edit the sketch and delete the current layer Sketch Figures and trace the next one in sequence. Then when you exit the sketch the part will rebuild with the next layer to SAVE AS.

When you're done with each layer bring them into an assembly and constrain them all to the same axes.

Layers Exploded.png LayersStacked.png
 

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DavidJ

Alibre Super User
Staff member
Depending upon which level product you are running, some options are

Option 1: Create a cone part (say circle extruded with draft). On sketch plane though cone axis draw a cutting line at material thickness from cone base, use thin wall cut to cut a very thin slice (say 1 micron) though the cone. Pattern the cut up the cone at spacing of material thickness. Use Remove Model Pieces from the Direct editing toolset to remove each slice. Feature suppression then allows you to have any slice visible. You could combine with configurations and have one configuration for each slice, or Save As for each slice to make new part.

Option 2: Start in an assembly. Insert a new part - extrude a circle with draft to material thickness. Exit that part, insert next new part, start on top face of previous part - project that face to sketch and use it as starting profile for a drafted extrusion to material thickness. Rinse and repeat as many times as needed. Save the assembly (and hence all the new parts).

Option 3: Extrude circle at diameter of cone base to material thickness, add chamfer to top edge of 'slice' to give required taper - this allows you to easily work out size for next slice. Repeat for each new slice in a new part, and then assemble.

There are probably a few other variations, and even methods I'd never have dreamt of. I'm often surprised by the ingenious approaches to modelling problems that members here come up with.
 
If you start with a basic sketch constructed of Reference Geometry:
View attachment 35172

Then trace each layer in turn with Sketch Figures, Revolve and SAVE AS:
View attachment 35173

After each SAVE AS edit the sketch and delete the current layer Sketch Figures and trace the next one in sequence. Then when you exit the sketch the part will rebuild with the next layer to SAVE AS.

When you're done with each layer bring them into an assembly and constrain them all to the same axes.

View attachment 35174 View attachment 35175

Hello Harold,
Thanks for the response. I like your reference geometry method quite a bit and can see myself using it for several applications provided the task is simple enough. I haven't utilized a SAVE AS workflow yet but I can really see some time saving opportunities from using one.

Screenshot 2022-01-21 122925.pngScreenshot 2022-01-21 124008.png
It is seeming to me like the Boolean method is the most straight forward way to achieve a slice for geometry with higher levels of complexity.
 
Depending upon which level product you are running, some options are

Option 1: Create a cone part (say circle extruded with draft). On sketch plane though cone axis draw a cutting line at material thickness from cone base, use thin wall cut to cut a very thin slice (say 1 micron) though the cone. Pattern the cut up the cone at spacing of material thickness. Use Remove Model Pieces from the Direct editing toolset to remove each slice. Feature suppression then allows you to have any slice visible. You could combine with configurations and have one configuration for each slice, or Save As for each slice to make new part.

Option 2: Start in an assembly. Insert a new part - extrude a circle with draft to material thickness. Exit that part, insert next new part, start on top face of previous part - project that face to sketch and use it as starting profile for a drafted extrusion to material thickness. Rinse and repeat as many times as needed. Save the assembly (and hence all the new parts).

Option 3: Extrude circle at diameter of cone base to material thickness, add chamfer to top edge of 'slice' to give required taper - this allows you to easily work out size for next slice. Repeat for each new slice in a new part, and then assemble.

There are probably a few other variations, and even methods I'd never have dreamt of. I'm often surprised by the ingenious approaches to modelling problems that members here come up with.
Hello David,
Thanks for providing these solutions! I just tried using Option1 with great success and speed:
Screenshot 2022-01-21 140423.png

Options 2 & 3 are similar in function to Harold's solution but go about it quite differently. Thanks so much for your help on this topic!

It is amazing to see the creative and different ways people use a set of tools to solve any given problem. I'm so grateful that the Alibre community is so welcoming and fosters such a positive learning environment for users.
 

HaroldL

Alibre Super User
Option 1: Create a cone part (say circle extruded with draft). On sketch plane though cone axis draw a cutting line at material thickness from cone base, use thin wall cut to cut a very thin slice (say 1 micron) though the cone. Pattern the cut up the cone at spacing of material thickness. Use Remove Model Pieces from the Direct editing toolset to remove each slice. Feature suppression then allows you to have any slice visible. You could combine with configurations and have one configuration for each slice, or Save As for each slice to make new part.
@DavidJ , At one micron thickness using the Thin Extrude Cut ends up being similar to using and Extruded Surface in SolidWorks. Very interesting use of the tool. And seems easier than my solution of using a Reference sketch. I don't use Thin Extrudes often but I'll have to keep this one in mind.
 

HaroldL

Alibre Super User
Not anyhow possible to put all parts using a same one sketch?
All parts do use the same sketch. Using the SAVE AS will create the parts so they all can be assembled at 0,0,0.
When getting the parts for the assembly, selecting all of them and inserting them at the same time will attach them all to your cursor at 0,0,0 so it appears that they are assembled. You still need to apply constraints in the assembly.

Do you have v24 so you can look at the package file I uploaded?
 

HaroldL

Alibre Super User
I came up with another method of using a base Reference sketch to define a part with slices. This uses the same basic approach as my previous method except that the vertical and diagonal lines are all segments with Collinear constraints applied to both. Equal constraints are applied to the vertical line segments and a dimension is applied to define the layer thickness instead of the part height. In addition to the base radius you can apply either an angle or a top radius dimension.

Then all you need to do is Window Select a group of Reference figures and convert them to Regular figures. Initially applying a Revolve to the first sketch selection. Afterward editing the sketch and converting groups of sketch figures as needed. IF you have Configurations ability you could create a configuration for each layer and have only one part file that can be inserted into and assembly as many times as needed for all the layers. Then activate the appropriate configuration in each "layer part" to build the assembly.

Here's a short gif anim for demonstration.

ConvertSketchesForLayers.gif
 
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