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I would like to see this feature implemented as well. There are ways around it but not applicable to all situations.
As a thought, even though this thread does not contain that many people who have requested this feature improvement that does not mean that there aren't more people who would gladly use an improved command. It's just that some people might not have the time or the will to actually post in here.
Additionally, it would be interesting to know why this improvement is not being actively considered as an improvement for future versions. Leaving aside the extra work to changing the code to allow for the improved functionality, are there any reasons why this request does not make sense? I mean from an engineering point of view and so on.
Thank you for considering the implementation of this improved functionality.
Solide Edge can do it as well if I'm not mistaken. And I wouldn't be surprised at all if the likes of Pro-Engineer, NX and so on, have this as an option as well. My guess it wouldn't be too hard for Autodesk to implement, so maybe it's a patent issue? Anyway, I still want this to happen for Inventor.
Having this feature with a depth up to, or offset from a face/plane would be nice as well - as opposed to having just blind depth. Currently can go up to surface, but sometimes I desire it to be offset from said surface selected.
Earlier on, I would have agreed with you, those additional options do make sense. However, it is possible to use a workaround to achieve exactly that.
Depth up to:
1. Create a workplane perpendicular on the surface where your hole is supposed to be. 2. Create a new sketch. 3. Use project geometry (or cut) to display the position of the hole start surface as well as the position of the surface (or any other feature needed to align the hole depth with). 4. Dimension the distance between surface and desired projected feature. Inventor will ask if you want to create a driven dimension, click ok. 5. Open your parameter window 6. Look for the driven parameter (has its own section, it's not in the user defined parameter section). 7. Rename the parameter (or not - but you do need the name of it) to something that makes sense to you. 8. When creating the hole in the hole window, instead of a value for depth enter the name of the parameter.
This will result in a hole with a depth that dynamically adapts to the changes in your model. This happens due to the project cut edges/project geometry you used in the sketch where you created the driven dimension to define hole depth.
(This might not work - I usually don't suppress features - in case you suppress any of the features that are used to project the geometry in the sketch)
This works in a top-down design, where you have the possibility to project geometry between individual solids that are later made into separate parts.
If you are working in an assembly, or in a single body part (where the feature you want the calculate the depth to is in another file), you can skip steps 1 through to 4 and start with step 5. This means that you will use a parameter to control the hole depth and that you will edit the depth values manually rather than allowing them to be modified dynamically as a result of changes in model geometry (if you change anything in your model that changes the value of the depth, you will have to edit the value of the parameter fromt he parameter window). If you have the depth value needed for the hole in another part file, it is possible to create a parameter that automatically defines the depth in the other part file and then you can import the parameter into the part file where you need the depth parameter. This will also create a depth that will dynamically adapt to changes in the part file you imported the parameter from. (if you do this however, it will not be possible to export any parameters from the current file into the file where you have imported the depth parameter from - Inventor does not like cyclic references)
For offset from face/plane, you can use the method above with slight changes in how you define your projected geometry.
Using the parameter way might be a bit complicated. But it has the benefit of reusability (you can use the parameter to create a large amount of holes). It also has some limitations (like if you remove/suppress the geometry used in creating the parameter) but the more you work with this, the more to adapt your process to this reality and thus will be able to avoid issues.
I prefer writing an essay. It is much cosier when you have all the information you need readily available to peruse at your leisure, rather than having to skip back and forth through a video. As such, if at all avoidable, I will not use a video, I will each time select an article. I am well aware that a picture is worth a thousand words. But it is also possible to have a thousand images fail to convey the simple message contained within a sentence.
I realize there is a way in which it COULD be done... but it is also the way in which it SHOULD NOT HAVE to be done. I don't enjoy wasting my time daily with menial things like this - when I know other programs can do this, and yet to MAKE it work in Inventor, I spend many more minutes, regularly, doing simple things like this... I like having simple model trees without all kinds of things implemented due to the inadequacies of the program... For editability now, the person later editing the model will have to go and fumble through all the random, miscellaneous, seemingly useless features - at first impression - to understand what the design intent was.
The especially frustrating/annoying part, is that they have half of the logic implemented to do what is desired by using the up to face... they just need to add the ability to add a dimension to do this offset. I avoid implementing a lot of design/modeling things that I am used to in other more advanced and common programs **cough SWx cough** because of the severe instability of the sketches, planes, features, etc. in Inventor - hence why I realize it can be done the manual way using a number of features, but avoid it because of the way Inventor handles feature relationships...
You mention that the "To" option - and the action of the face selection - should have an offset dimension. In other words, when you select the depth of the hole you would like to select a face as a point of reference and then enter the distance the hole feature's depth should keep from this face. This would subsequently mean that if the selected face is moved, the offset will automatically alter the depth of the hole.
It is possible to achieve this offset you require in at least two ways I can think of right now. The first one is to create a sketch and project the required face (the "to" face) on it, then create a driven dimension between this projection and the projection of the hole's starting face. This dimension can then be used as a parameter from which the offset is subtracted: hole depth=todrivendim-offsetval.
It is also possible to select the "to" face, create an offset plane from it and then select that plane as a "to" for your hole depth.
But both my solutions as well as your scenario provide Inventor with the possibility to break the model. If the face (your way or my way) used for the "to" selection is suppressed or deleted, the hole feature will break (because the "to" selection is now an orphan) and all other features that depend on either the face or the hole in question will stop functioning until the issue is solved. It can be solved easily, you can just edit the hole feature and either select another face as a target for the "to" option or simply enter value (or parameter).
As such, I would suggest avoiding the "to" option altogether and instead using parameters to establish the relationship between the hole depth and other surrounding features that might have to be taken into account when establishing the depth of a hole. User defined parameters (manually set up as new parameters instead of naming the parameters whilst creating a sketch - or feature) are not reliant on model geometry and therefore will not break the model if features are suppressed or deleted. The better you know the model you are working on, the easier it is to know which dimensions are vital for the design and special care can be taken in their definition and usage. If you are just drawing a concept, then you have a problem... but that's Inventor. Whenever I stumble on that, I usually save my file and start a new file/project and start from scratch. Doing this might cost a bit of extra time but in the long run, it will ensure the adaptability of your models.
I agree. Inventor has its own ways of doing things. And when you start using Inventor, it can be frustrating because you know what you want your model to be like, you just can't figure out the best way for Inventor to take you there. I wish I could give you a shortcut past this stage, but other than power through and get to really know Inventor, there is none. You mention SW. You are fortunate. My only CAD experience before meeting Inventor was SketchUp. So... erm... parametric CAD design vs. something I would rather call a concept tool... not the ideal mix 🙂
