Hole ? - which is a better way to add the feature?

[ColinPearson]

So, I'm sure anyone that knows Inventor will be able to tell, but I am new to it. Many years of CAD but about a week in Inventor.

I've been trying all morning to add holes to a part. My idea was to make a sketch, extrude it and then add a hole and pattern as needed. The linear option was no good to place the holes b/c my sides are not square with each other, so I when back and edited the sketch to place a pair of construction lines crossing at my intended hole center. I place a Center Point at the spot, but when I went to add a Hole feature later, (trying From Sketch and By Point), Inventor didn't pick up the Center Point. I finally googled enough to find that I could click on Sketch1 (which Extrusion1 is based on and through which Hole1 will go), click Share Sketch and now I can add a Hole feature using the From Sketch option. Questions are as follows

1) Why can I not use the endpoint or intersection of the construction lines to place a Hole using the On Point option?
2) Do I even want to do this? Is it better to make a Sketch1 and a subsequent Extrusion1 and THEN create a new sketch on the face of Extrusion1 and then base my Hole feature on that? I guess I'm asking should my reference marks be contained in that most base sketch or is there a compelling reason to separate a sketch that will only define a feature from the sketch that defines the base object?

 

[mcgyvr]

1) "on point" is intended for work points.. not sketch points
2)No don't do that.. In general.. Its always best to make the shape a sketch/extrude.. then another sketch for each hole size,etc... In general each feature gets its own sketch..
And until you know any better thats how you should continue.. There are times when you can share sketches.. But in general don't..

If you can provide a the details (2d drawing or whatever) I'd be happy to model it up as I would (as an expert in Inventor) so you can see how it should/could be done..

 

[ColinPearson]

@mcgyvr, thanks for answering this one too! I've got it modeled, but I shared the sketch. Based on what you said, I guess I should project the shared geometry to a new sketch and then unshare the first base sketch and finally re-place the hole feature on a point in the new sketch. Anything else you might see? Thank you

 

[Sparweb]

Colin,
What you did is OK and similar to what I do often as a user of Inventor for 3 years. One modification though...
If the holes in the face are intrinsic to the function of the face of the part, and can share the same sketch plane, then I would do this:
[ul]
[li]Draw the sketch of the face and use construction geometry to locate the holes as points.[/li]
[li]The first feature to use the sketch is the Extrude feature, and then by sharing the sketch and making it visible the Hole command can use it too.[/li]
[li]If there are points on the sketch, the Hole will automatically place holes at all the points, which saves time.[/li]
[/ul]
I find that one "master" sketch that generates numerous features (instead of transferring geometry between multiple sketches) is much more resilient to changes you make to the part models later, and keeps more of the design features in one place and in context. This is not what my Autodesk training taught me. There's a lot of talk about design intent and proper parametric design procedure, but neither I nor my coworkers worship that stuff, and yet all our parts line up.

STF

 

[ColinPearson]

Thank you SparWeb... delay due to me intentionally leaving the computer at home for weekend at the beach. I've also been told that basically every feature should get its own sketch. I use between 50 and 200 layers in a typical CAD dwg when planning a large job, with new layers for every option, phase, scenario, etc. so I do know the benefit of carefully 'compartmentalizing' the design data so the waters don't get muddy. On the other hand, I'm tempted in this case to share that construction geometry like you said. I'm only two weeks into this thing, so I know I've got a lot of mistakes to make and swearing to do!

 

[Sparweb]

Good, at the very least you know what a layer is for in ACAD. Many kids now haven't used 2D CAD for real (and I won't mention the graphite stylus CAD from generations ago) and this may be the reason why parametric CAD instructions emphasize the sketch/feature structure the way they do.

Of course, don't sketch EVERYTHING on one primordial sketch, but if for example two different fastener rows must be placed in relation to each other, then model them on the same sketch, and that way you can design the locations of all of the fasteners together, and in their proper relationships before creating multiple hole features.

STF

 

[ColinPearson]

I never particularly like dealing with architectural drawings, but at a previous civil engineering firm I worked for, it was a regular occurrence. I did notice how many layers they always had and took that away for myself. There's no way that I could function without using the pretty detailed layer control system I've made for myself. When I moved to this job (turnaround construction, mostly petrochem refinery work), the two engineers above me would literally just start a new drawing for every option, or worse, just copy the entire geometry over a few hundred feet in the same dwg and change layout, options, etc. It made me crazy!

 

[Sparweb]

Years ago, I was tutoring an architect, who needed help with AutoCAD having only drawn by hand in the past. One day he showed me some of his work where he had copied several rooms out of a commercial building floor plan off to the side in the model space. He wanted me to show him how to get the changes he had made in the copied rooms back into the original rooms. I was dumbfounded. You just don't do that, I told him. Why, he asked innocently. If you wanted to change the rooms, why not change the rooms in the original drawing? He said he wasn't sure he would make the changes right.

So drawing change strategies and revision control were the subject of the tutoring that day.

STF