Streamlining adding void features to lots of bodies?

[cmcdonaldXHNC9]

I'm building furniture/cabinetry that can best be described as Ikea like as I'm using dowel pins to hold most of it together. So I need matching features on joining components. I'm cutting on a 3 axis CNC router and I've designed and printed a jig to drill the holes perpendicular to the sheet. I put a notch on the edge where the holes need to be drilled and the jig keys into that notch. 

The problem I'm having is that it's extremely tedious and time consuming placing all these features.  My current workflow uses a component that has bodies for each of the features to be cut and a sketch to give me a corner point to reference to. 

Current work flow is:

- Move/Copy cutting component

- select point to point

- Select point on sketch

- Select destination body's corner

- click create copy

- select free move

- click set pivot

- click on corner  

- click the checkmark 

- rotate each axis to get into correct orientation

- Redo Point to point move, if I needed to flip the cutting component

- Set offset from corner if needed

- combine with body A

- select the three bodies in the cutting component

- click ok

- Turn off visibility on body A

- Turn on visibility on body B

- combine with body B

- select the three bodies in the cutting component

- click ok

(Sometimes I do the combine for a bunch at a time, but it's easy to miss cutting bodies)

It's many steps and I have hundreds of these to do. I'm looking for some ideas on how to do this in fewer steps. There must be a better way to get the cutting component in into orientation. In an ideal world I'd just select a face and a corner and the cutting component would appear in the correct orientation. 

Also a better way of selecting all the cutting components bodies for the combine step. It's tedious both in 3d space and in the browser to select these.

The whole using combine to cut process seems a long way around in the first place. I really wish we could create void form bodies like the void form extrusions in Revit. 

I've attached a screenshot of the simplest situation. But of course they get more much more complicated. The key part is the relationship between the holes on one side and the notch on the other must be consistent. I always cut finish surface down on the CNC router, so the notches are all on the back/inside of the finished pieces. 

Any ideas on how to do this in fewer steps? 

[TrippyLighting]

Please attach you design in .f3d format.

Your description indicates that you are missing basic concepts (patterns, joints) and it is often if not always easier to explain these concepts on an actual design.

[TheCADWhisperer]

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@cmcdonaldXHNC9 wrote:

Any ideas on how to do this in fewer steps? 

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I would use Autodesk Inventor Professional - iFeature for this (or even more sophisticated the Punch tool with a trick to place as simply as placing Hole features).

[cmcdonaldXHNC9]

I do use patterns when the pins are on the same plane, orientation and with regular spacing. But most of the time they are not. Think of something like a park bench where each of the planks is at a different angle. 

When I have a number of internal members that are all the same, I'll make copies of the cutting component as sub components and then pattern the internal members. The problem comes when it's time to combine(cut) with the end plates, it's somewhat tricky to select all the cutting bodies. I had much frustration with this last week. I had mirrored a few of the internal members and suddenly the cutting component bodies stopped working with the combine tool. 

The other issue with that method comes when you need to add new features to one of the patterned components. You must copy and paste new... Why haven't they added a make unique function...

Joints could work in some situations, they may be faster at getting the cutting component into the correct orientation. I'll have to give that a try. 

I can't attach the actual files as they contain design work that I do not own.

[TrippyLighting]

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@cmcdonaldXHNC9 wrote:

I can't attach the actual files as they contain design work that I do not own.

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Then please create a dummy assembly that exhibits the same problem.

[jeff_strater]

I'm not sure I completely understand your process here, but it seems like you might be able to use a template component or components to do some of this.  Define a component that has bodies that you would use to cut into the target geometry.  Define Joint Origins on that component to help you place it on the target.  Use Combine to remove material from the target.  If you uncheck "Keep Tools" in Combine, then those bodies would be removed by the Combine.  Or, you can Remove the entire component when you are done with it.  Component Pattern could be used where there is a series of these operations in a regular pattern.

[cmcdonaldXHNC9]

Here is a quick and dirty example. I usually wait until I go to arrange to convert to components because I don't want to paste new every time I need to copy a unique body. Pretty much any where two parts meet I need the pin holes or the notch. I put a few in of the cutter components just across the bottom. In the real version, most of the studs have unique features, so copying components does not work great for that. Where the brace components go between the studs the holes need to be cut into the adjacent studs for example and the placement of the braces varies greatly. 

Currently it's taking me longer to place the cutting components for the pins than model the whole thing.  A fraction of that time again to setup the tool paths. It's a major bottle neck in my process right now.

I tried using joints, I find it tricky to get the orientation right. It doesn't really like working with the sketch edges. Works fine in some orientations but not all. 

[cmcdonaldXHNC9]

That is essentially what I'm doing. It's just getting the cutting(template) component into the right orientation that is really tedious. Also selecting the bodies inside that component from the combine dialog. It really should select the bodies from within a component when you click a component in the browser. 

If we could set the bodies as void(like a hole but with arbitrary shape), it would reduce the number of steps here greatly. It feels like a hack to have to use the combine tool to do this.

Joints kind of help but they often don't work like I expect them with the components meeting in the wrong orientation. Is there a modifier key or something I'm missing that cycles through the orientations or something?

[jeff_strater · Accepted solution]

"If we could set the bodies as void(like a hole but with arbitrary shape), it would reduce the number of steps here greatly. It feels like a hack to have to use the combine tool to do this."

That is pretty much what would have to happen with a "void" body - it would use Combine to do exactly that - subtract the void from the target.  So, yes, using Combine does add one step, but it does not, IMO, seem like a huge step to me.  Eye of the beholder, of course...

"Joints kind of help but they often don't work like I expect them with the components meeting in the wrong orientation. Is there a modifier key or something I'm missing that cycles through the orientations or something?"

That is why I suggested the use of Joint Origins.  Adding Joint Origins to your component allows you to specify exactly how the component will connect to other components.  If you are using Joints with just geometry references, yes, the orientations and adjustments are limited.  The intent of that workflow was always to cover the most common/80% set of cases, where creating the Joint Origins would be more trouble than they are worth.  However, for cases that fall outside of those, using Joint Origins can give you a lot more control.

[TrippyLighting · Accepted solution]

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@cmcdonaldXHNC9 wrote:

That is essentially what I'm doing. It's just getting the cutting(template) component into the right orientation that is really tedious.

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Joints form the assembly menu are designed to do this. But it can indeed also be tedious.

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@cmcdonaldXHNC9 wrote:

 Also selecting the bodies inside that component from the combine dialog.

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In my experience, this is the most tedious and repetitive task. This very nifty plugin makes this super quick work!

Cut/Join by Componet.

[cmcdonaldXHNC9]

Also a bug with the combine tool, once you select an instance of a body within a component pattern the other instances of that body go invisible. You can still select them if you know where they are, but they don't show on screen. This has been a bug for a while, like years.

[cmcdonaldXHNC9]

Joint origin seems to work well, now that I have it figured out. I was using a sketch for this before, this works better. Only annoying this is how hard it was to select the Joint origin with the sketch geometry there, it was selecting the sketch points rather than the origin. Turned the sketch off and its working good now.

Thanks

[cmcdonaldXHNC9]

That plugin looks amazing. That is going to save me so much time.