Turning slot or dado on or off based on parameter

[Anonymous]

Hey guys - Very new to Inventor and am trying to work through it myself.  I have a question regarding a dado or slot for a shelf in a base cabinet.  I have set up a rule where a feature (Shelf) can be turned off or on and everything works fine.  However, I have another part to the rule that I cannot figure out.  I have a multi value list in the paramaters for "Shelf_End" - the values being "Butt joint", or "Dado".  Since I drew the sketch for the shelf with a dado, that portion works fine if "Dado" is selected.  However, if "Butt Joint" is selected then the dado or slot remains in the adjacent piece or feature.

How do I write something in Ilogic where if the "Butt Joint" is selected then the dado disappears and there is no void.

I greatly appreciate the help in advance

Mike

[Anonymous]

Well Mike,

I could probably use a file or two to help visualize the issue. Maybe even some screen shots now that I think about it. But it sounds really simple if you're already using iLogic. Sounds like a:

If Shelf_End = "Dado" Then

Feature.IsActive("Dado") = True

Else If Shelf_End = "Butt Joint" Then

Feature.IsActive("Dado") = False

End If

But again... that's my take on it given what I can tell from your question. I'm happy to help further but I may need more to work with. Sometimes having the model itself is the absolute best way to address the situation.

Thanks,

[Anonymous]

Will Mann

Thanks for replying to me and offering your help and expertise.  I have attached the model for you to review. 

I guess I was on the correct path because I tried what you said before and it still didn't work.  I'm thinking that it is something in how I did the sketch for the actual shelf.  Since I trimmed the actual sides of the cabinet where the shelf would intersect - or where the dado would be to receive the shelf - I'm guessing that is why it remains even if I select the "Butt Joint"

Here is the model.  Let me know if there is anything else I can send you to help.

I really appreciate the help

Mike

[swalton]

Two choices:

1. Make your dado cut a separate feature, not part of Extrusion 1.  Then suppress/un-suppress this feature as required.  This would be my typical method.

2. Make a feature that fills in the dado cut you made in your first feature.  Then suppress/un-suppress this feature as required.  I don't like making features and then filling them in, seems a waste of time.

Btw, any reason that the toe kick does not start on the XZ plane?  If you did that, the measurement from the XZ plane to the top of the cabinet would be the same as the installed height.  That might be a useful convention as you populate your room with several cabinets, counters, etc.

[Anonymous]

So after quickly looking over the model, I'd likely go with swalton's second suggestion:

Create a feature that turns the Dado into a Butt Joint and suppress/unsuppress that feature based on your options.

I think that'll be the way to go. And you might not even need iLogic for that. Check out right clicking the feature and editing it's properties. There are suppression conditions there that may allow you do to what you want to do without iLogic.

Hope this helps.

[Anonymous]

Swalton 
Thanks for the reply and help.  I am trying to do what you suggested in your first suggestion but it is not letting me cut a void.  I'm assuming that I create a sketch and then do an extrude cut feature. But nothing happens. It actually doesn't even let me hit Ok to see if it works. What am I doing wrong?

Again I appreciate the help

Mike


Sent via the Samsung Galaxy Note® 3, an AT&T 4G LTE smartphone

[swalton · Accepted solution]

Here is my edited part. 

Here are my steps:

1. Added two lines to Sketch 1 that close the dado cut on each side of the cabinet.
2. Ran Sketch Doctor to make sure IV understood that I had closed the two dado cuts.
3. Edited Extrusion1 and selected the closed boundary of the dado cut in Sketch1.  This filled-in the dado in Extrusion1.
4. Pulled the EOP up below Extrusion1
5. Created a new extrusion and selected the closed boundary of the dado cut.  Selected Cut and Through All.  I did not have to select a solid body, because at that point in the model tree, there is only one.
6. Renamed the feature to Extrusion1 Dado.
7. Pulled the EOP down below Extrusion2.
8. Edited Extrusion2 and selected the closed boundary of the dado cut in Sketch1.  This filled-in the dado in Extrusion2.
9. Created a new extrusion and selected the closed boundary of the 2nd dado cut.  Selected Cut and Through All.  Selected solid body 2.
10. Renamed the feature to Extrusion2 Dado.
11. Pulled the EOP down to the bottom of the model tree.

You could also put a single dado cut below Extrusion2 that affects Solit Body 1 and 2, but I don't know how that might affect your later workflows.

I did not look at the ilogic or conditional suppression of the dado features.  Will has a better handle on that type of modeling than I do.  Most of the time I design one-off machines and automation like this seems like overkill.

[Anonymous]

Swalton

I am sorry for taking so long to get back to you.  Everything seems to be working great.  I really appreciate the help.  You guys on here make it alot easier trying to navigate this program by myself. 

Again I appreciate it.,

Mike