constraining depth of H-blocks

[Guest Orlik]

Imagine this simple example:

I created a structured part.
I put a Block from the catalog. Then H-Block on top of it.
I changed depth of that hole with a triball handle, so that the hole goes throught whole part (z-axis).
I edited a sketch of H-block so that the block have always thinkess 2mm, even if change x,y dimensions of main block. GREAT.

But when i change "z" dimension of the main block, then depth of H-block is not updated automatically. 

Question: How to constrain H-block to always hold it's depth through whole part?
 

[SSIMMONS]

Can you just use the shell command and set the open faces and uniform thickness of the shell instead?

- Spencer

[Cary OConnor]

For the Depth of the H-Block, just edit the feature and change it to a Through All depth setting versus an input depth (or blind). That will maintain it as a through cut. 

The same can be done on an innovative part as well. Not sure if you have a specific reason to use structured parts.

Cary

[Jonas@Solidmakarna]

When you [Shift] snap a red round Sizebox handle to another face (lights up in green) you do not create a relation/constraint. Instead that process (snap) will "only" create a number for the extrude to stop at, nothing more. This is a basic and important part of IRONCAD, the numbers you set will never change "automatically". For me this is crucial and I trust the system on this.

However, If you want to set these kinds of relations you can do it in several different ways. For an extrude to go all the way through the part you can right click on the extrude feature (which might be an H Block) and set the "Forward End Condition" to go through the whole part.

I think it is also important to know and understand that the reason why we don't want to use constraints and relations is because there are other types of tools and workflows in IRONCAD which doesn't exist in other 3D CAD systems! "Automatic" means "a rule that someone has decided" and you usually cannot bypass this in an easy way. By skipping this "automatics" and using manual tools (which are really fast) you have more control!

[Malcolm Crowe]

Attached are a couple of videos demonstrating a couple of methods of how to maintain the position of one feature (Intellishape) relative to another. I have used the example of constraining the bottom of a blind hole within a block, where I want the position constrained relative to the base of the block. Sorry if this isn't exactly what you are trying to do.

1. Constraining Features by Sketch Position - Structured Parts

2. Constraining Features by Smart Dimensions - Innovative Parts

Note that for "Smart Dimensions" to behave as constraints they need to be "Locked". This is demonstrated in the second video.

When working with "Structured" parts, understanding how to position (constrain) the underlying sketch positions relative to planes and other features is critical.

Malcolm

Constraining Features.ics

[Guest Orlik]

These answers are very helpful. Than you!

One more question. If I double-click on that dimension visible in 0:24 of the second video, a window shows up.
It looks like I could also change that dimension from there. But when type in a different value and click OK, or apply and then OK - Nothing happens. Is there any use for that window? How to use it?

PS: I know about function shell, but I want to learn basic manipulations of IC.
 

[Cary OConnor]

Make sure when you created the dimension, you have the IntelliShape feature (yellow) selected. If not, it may apply it at the part level which in that case you can't edit or drive anything since it is really a reference dimension at that stage. One setting you may want to change in the Options is to apply the Smart Dimension to the selected shape (Tools-Options-Interaction, Under 3D Smart Dimension/Constraint it is the 3rd option "Keep Selected Shape as Affected/Owning Object when creating dimension"). 

Cary

[Malcolm Crowe]

In the attached video I am editing the value of the Locked Smart Dimension.

Select the the Intellishape that belongs to the Smart Dimension. Double-click on the dimension and the dialog box opens. Change the value and select OK. This can also be done by right-clicking on the Smart Dimension under Constraints in the Scene Browser (History Tree).

Malcolm