Inserting existing models and using as a tool

[Anonymous]

Can anyone please advise how I may be able to use an existing model, import it into the workspace and use that imported model as a tool to subract from the model I'm working with?

The actual application is a spindle adaptor where I have an #4 Morse Taper body that will become an adaptor for a W20 collet. I have modelled both and would like to import the W20 collet and use that to punch out the #4 Morse Taper. I can import the collet, but I'm not able to move it around, or even select it after initial import is completed. I then don't know how I would use that to subract from the original model. I'm sure it will be quite straight forward, but I'm not sure how.

Thanks

[jeff_strater · Accepted solution]

This should be relatively straightforward.  Once you have Inserted the collet, there are several tools that you can use to move the inserted component:  Align, Move, or even just dragging around on the screen.  Once you have it in the correct position, use Combine to perform the cut operation - select your #4 Morse Taper body as the target body, the collet as your tool body, change the operation to "cut", and you should be all set.

Here is a small screencast showing how to do it in a very simple case:

Jeff Strater (Fusion development)

[Anonymous]

Thanks Jeff, I agree it was easy and why I was frustrated, however the issue was I couldn't select the tool body. It turned out that even though the whole body was selected I needed to check the appropriate box in the move command. I guess I wasn't expecting to need to do that but caught it in the screencast. It was driving me crazy as it seems as if the two bodies are handled in different ways by move. eg even with both selected and in blue, upon initiating the move command the tool body will grey back out again.

[jeff_strater]

This is admittedly a sometimes confusing area of Fusion - the notion of different types of selections, and commands which can act on the different selection types.

So, when you say that the entire body was selected, my guess is that you selected it using the window select command, while no command was running.  Is that true?  If so, then I understand the behavior that you are seeing a little better.

In Fusion, there is a hierarchy of items in the view.  From the bottom up:  Faces, Bodies, and Components (an over-simplified view, there are lots of other things, too, but I suspect that these are the relevant objects to your case).  A body is a collection of faces, and a component can have zero or more bodies in it.  Fusion can select any of these objects.  You can see what all objects are possible to select by looking at the selection filter:

Now, there is a special problem with the Component/Body/Face hierarchy:  Neither a Component nor a Body really has any geometry of its own - you select a body by selecting its faces, and that selection is "promoted" to a body selection if the Face filter is off and the Body filter is on.  The same is true for Components (I'm not sure if you are using Bodies or Components, but the idea is the same).  By default, when no command is active, and you select geometry, you are really selecting faces.  Even if all the faces of a body are selected, we still consider them face selections (we've had lots of internal debates on this topic over the years whether this is desirable...)  So, if you try to select the body using window select before the command is active, you will actually be selecting faces.  But, the Combine command cannot act on faces, only on Bodies, so it discards those face selections.  But, if you invoke the command first, the command knows it can only operate on Bodies or Components, so it is able to adjust the selection filter to promote Face selections to Bodies.  You can tell by looking at the selection filter when Combine is active:

I admit that this can be confusing at first, and non-obvious.  I'm only explaining how it works...

I hope this helps a bit to clear up some of the mystery.

Jeff

[Anonymous]

G'day Jeff, thanks for following this up. I'll need to read through your explanation a few more times as I think you've made some very important distinctions there, but in the meanwhile wanted to answer your questions in regard what I was doing.

The tool was derived from an existing model of a W20 collet, and rolled back to get rid of things like the thread and registration groove. It was then copied into the existing workspace using the "insert into current design" command. At that point it is highlighted and is set up to be moved to position. However let's say I now need to do some other sketching, say to create a point to move to, I'd select it by dragging a select box around it and using the move command either by right clicking or the Modify Menu. It would un-select and could only be selected by checking the Component option in the Move dialogue. The issue was because it seems as it is linked back to the original model it's treated as a read only Component, and not a body. I could move it by either just treating it as a component with that option selected, alternatively breaking the link to the original model and then it becomes a body again.

I THINK I have that all correct, no guarantees however!!!

[jeff_strater]

Thanks for the explanation.  You are correct that because you are inserting it, the component is read only, and that may affect some operations.  

However, I think the key point, to what I was saying above is this part:  "I'd select it by dragging a select box around it and using the move command either by right clicking or the Modify Menu. It would un-select and could only be selected by checking the Component option in the Move dialogue."  I think this is what got you.  This is where the Face vs Component selection is confusing.  When you box select the component, outside of a command, it really just selects the faces.  And the Move command doesn't know what to do with faces, so it dumps them.  Admittedly not great behavior, but we're not really sure what we should do in those cases.  Most likely, the right answer is to promote those to component selections.

But anyway, I think you are moving in the right direction now.  And, we have some real-world feedback that we can use to maybe improve the behavior.

thanks!

Jeff

[Anonymous]

Thanks again Jeff. Obviously you've been most helpful, however I think we both got something out of this. I'd agree with you, just dumping something, in any application, without a warning isn't cool. Even a warning that may be understood only by the developpers isn't much better, and some of the warnings are a bit criptic to those of us new to the program or indeed the whole 3D CAD field.

To dumb it right down, if I box select something I'm not doing so for a laugh and a giggle, it's because I want to select it to do something (in this case move it). If I can offer an analogy; when cars were first relesed the people driving the vehicles were typically mechanically savy and knew the mechanics behind the vehicle and how to maintain the mechanicanism. These days we don't need to know that, we get in our cars, push the start button in many cases, and off we go. There's an amazing amount of complexity happening around us, but we're unaware of it. So it should be with applications like Fusion. I can't even comprehend where anyone would start in developping a CAD program, and I genuinely admire those who make it happen. But the botom line is, just like my modern car, I don't need to know. In this case if I select something I want it selected, and shouldn't need to think of what it's "made of". So I think your thinking of it along the lines of "promoting" a selection is the right thinking and I would encorage the development team along the same path. That thinking doesn't mean making the application more basic, quite the opposite, it's a matter of harnessing the power in an intuitive interface; what is the person wanting to do here?

Something for the development team to ponder: How can we take a person to their destination in our vehicle without that person needing to be aware of the complexity of the vehicle itself?

Thanks again for the help. More dumb questions to follow!!!