shapes in parts

[David Thomas]

Is it possible to extract a shape back out of a part?

 

For example:

You have two blocks in two parts - one part is marked for subtract material

Do the boolean so you have one part with two shapes in it.

If I have forgotten to make a copy of the subtracting part which I now need to subtract from another part, what can I do?

 

Thanks

[Mike Allen]

You can drag the shape into a catalog, then drag it onto a new part. I always make sure that the anchor for the shape is in a convenient place for positioning it (the center of a curve, an endpoint, or a midpoint, for example) before I drag it into a catalog.

 

 

[David Thomas]

I just tried to drag the shape into a catalog. It won't let me do it though. It seems that you can only drag from the drawing and not the part tree. Subtracting shapes cannot be drilled down to in the drawing so I am unable to drag it into the catalog.

 

Any ideas?

[B. Ludin]

I have no problems drilling down to subtracting shapes. I can also select the shape from the browser and then select it from the scene, if necessary.

 

Beat

 

 

[Chris Lohman]

Sometimes when my shape is buried, I'll have to select it in the scene browser and then drag it from the scene. You are correct in finding that you can only drag it from the scene. Sometimes if my shape is very buried I'll have to suppress other shapes to get to it.

 

In your situation David, if the catalogs are difficult for you, there is another way around this. You can duplicate the entire part (copy/paste) and then in the second part you can delete all of the shapes except for the one(s) that you want to keep in their own part structure.

 

 

 

[Mike Twining]

Just a side note, if I were you I would avoid Boolean operations like the plague (so they say). You can get the same functionality by using an array of "H" parts (or negative shapes) which will allow you to control the geometry and maintain the "intelligence" of the different parts.

 

MikeT

 

 

[David Thomas]

Mike

How do I make a part into a negative part and make it subtract from another part without doing a boolean operation. Even when you drag a hole pattern out of the catalogue it goes into the part as a shape.

 

I have attached an example. I want to get the shape "subtracting" back out of this part to use elsewhere.

 

Or, for my next drawing, make it subtract from the block without doing the boolean.

 

example.ics

[Chris Lohman]

David what I think Mike is saying is that you model the negative using negative shapes to begin with (which is a good recommendation), not a positive shape that you somehow switch to a negative. See the attached for an example of said suggestion which contains your original part, and then a version of it that I rebuilt using intellishapes. Expand the parts in the scene browser to see the differences.

 

Below is an explanation of the avoiding booleans statement.

 

Booleans are far more mathematically complex than intellishapes are. So the more booleans you use; the more difficult the geometry will be to process; and thus the longer it will take to process. Booleans also create geometry that is not as flexible as an intellishape:

 

So when you use a boolean you:

 

1) Lose the flexibility of IRONCAD's intellishapes: Which is a loss of one of the major features that makes IRONCAD so easy to use. (You still have the profile handles and profile editing though, so all is not lost after a boolean)

2) You could kill your processor IF your booleans are significant.

 

David in your simple example; a boolean isn't a big deal for the processor to use. You lose the flexibility of the intellishapes; but you can just as easily go back and edit the original cutting tool and then re-boolean the part in your simple example.

 

So using boolean or not really becomes an issue once your geometry grows to a significant (enough) level of complexity. Think of a plastic cavity with ribs and bosses...you could model the cavity, ribs, and bosses, in 3D and then just cut them from a block using boolean: Or you cut the cavity in the block using intellishapes (or a shell) and then build the ribs and bosses into it using regular positive intellishapes. In my cavity example, that single boolean could define almost all of the geometry in your part; which would make it difficult to go back to and edit and would also make it very very CPU heavy. The intellishapes calculate much faster and they're easier to edit than a boolean so you could win twice by modeling in the negative to begin with.

 

Of course it's often very difficult to visualize and model a negative shape: So ultimately you should be using IRONCAD to work as fast and as productive as is possible for you. So if you can model in the positive and boolean that shape much faster than working with negative/intellishapes; and you don't think that you will need to make many (if any) design changes and it isn't killing your CPU: Then please use IRONCAD in a manner that makes your job the easiest and most productive.

example2.ics

[Chris Lohman]

Oh and David to answer your initial question; if you cut a negative shape using a boolean; aftercutting you delete your initial cutting tool, and then at a later date you need to get that tool back: Your only option is to perform another boolean in order to rebuild your tool. Unfortunately once you get into boolean world you lose some of the most flexible features of IRONCAD; the intellishapes: So editing that rebuilt tool must be done at the profile handle/profile level, or by adding positive or negative intellishapes back onto the cutting tool.

 

 

[Mike Twining]

David-

One more thing to add (to answer one of the questions you asked). In order to have the "H_Block" and "H_" whatever work as a cut and not a positive shape (as your are seeing) you need to drop these items onto an existing positive shape. As an example, if you want a block with a hole in the middle, you first drop a block into the scene, then you select the "H_cylinder" (or various other tools available for making holes) from the catalog and drop that part ON TO the original block. This will cause the "H_Cylinder" to become a feature of you part (you will get a little + sign next to the part, which you can expand and see all the features).

 

If you drop Shape2 onto an existing Shape1, then Shape2 will be a feature of Shape1 (1 part with 2 features).

 

If you drop Shape2 onto nothing in the scene, then Shape2 will become its own (new) part.

 

Hope this helps you out!

 

MikeT

 

 

[Mike Allen]

Try this catalog. I made H-Intellishapes to match the cutaways on your part. then I aligned their anchors to the corner of your part and dragged them into the catalog. When you drag them onto the corresponding point on the new part, just align them with TriBall.

 

 

 

CustomSubtract.icc

[Chris Lohman]

Ooh Mike...good call; nicely done.

 

 

[don_temple]

While I understand Booleans can be very CPU intensive, a major benefit of CAD design is modeling your product once and using that model for downstream design and production. Using Booleans is often the only practical way to carry a design through the CAE pipeline.

 

To be truly efficient CAD programs must allow re-use of models for many operations and the shapes must remain associated and editable.

 

Given the current implementation of Boolean tools in IronCad its easy to see why we're so stuck on this issue. The "Set part operation" and "Perform Boolean" strategy is easy for novices to follow but it prevents advanced users from using models in the many ways they need to be used in tool and production design and it forces us to break associativity with our parent models.

 

There was a poll a while back about a new feature for version 7 that seemed to allow Booleans with linked solids. Is that functionality in our future?

 

Product & injection mold design.

www.QuickCAD.biz

[Chris Lohman]

Don we had a version of that boolean/linkage stuff in older revs but it was causing catastrophic failures in the models so we had to pull it out to prevent mass data loss. But even though it was pulled, it's not forgotten. It is such an increadibly complex feature for us to build (and keep easy) that we will have to put much more work into it to insure that it could never cause problems. So we probably won't see that added back into 7.0; but there remains hope for us to have that functionality in the future.