Centering Hole on Rectangle

[fsonnichsen]

This is similar to a prior question and reflects my difficulty with Construction lines on both sketches and designs. I never seem to get the "affinity" that is needed to snap objects into place.

  I pared down the problem into the attached f3d.   I want to place a hole, centered, on the rectangular appendage.  I have purposely placed a hole, offset, to show what I mean. I have construction lines at both the Sketch and Design levels. Front or back-I cannot cause the hole to align. 

  I probably can work around this by breaking up the sketches, extruding separate parts etc but it seems like a convoluted workaround.

  Any thoughts appreciated

Fritz

[TheCADWhisperer]

What are the Axis for?

White dots?  Not good!

Redundant line over top of another line?

Video >> to follow when it is done compiling.<<

[fsonnichsen]

Thanks. While we wait for your compile:

Why do I get the white dots? These seem to result from piecewise construction of the sketch(sometimes) -but I don't know how to join them.

Regarding the redundant line--I know it is invalid but I don't see it in my sketch---do I need to turn on some type of option?

FS

[TheCADWhisperer · Accepted solution]

>>See Video<<

[HughesTooling]

First question, why are you drawing the shapes in random places? Far easier if you draw at the origin and use it to constrain the sketch position.

Not sure why you're using 2 components if you're going to combine them into a single body.

Here's a screencast fixing your sketch and constraining it to the origin. You should always aim to fully constrain the sketch so it shows the lock icon.

The reason I drew the construction lines at random places then added a midpoint constraint between them is it allows you to modify the rectangle without losing the centre point. Example below, trimming a corner away. If you pick the midpoints of the lines or corners for the construction lines any edits to the rectangle will lose the centre point.

Mark

[HughesTooling · Accepted solution]

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@fsonnichsen wrote:

Regarding the redundant line--I know it is invalid but I don't see it in my sketch---do I need to turn on some type of option?

FS

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I hadn't spotted that either. I guess I should have tried dragging the white dot as it make it pretty obvious. Also shows the danger as you used the midpoint of this line for your construction line to find the centre. If you left click and hold on the line at the top you get a list box that shows there are 2 lines there.

[fsonnichsen]

OK--thanks for the Video--I guess the bottom line is this:  One needs to constrain everything properly in a sketch to use it as guides for further objects.

   Usually I follow that rule (I think you mentioned it a long while back) but I sometimes get a little sloppy and did not realize the importance in this case.

  Your time is appreciated!

fritz

[fsonnichsen]

Thanks Mark--Again as CadWhisperer pointed out, I guess I have to be sure that everything is constrained in order for it to work.  You comments on the midpoints make sense and are appreciated.

  Regarding your questions:

1) Actually my drawing was reduced to make it simple for the forum-my final design probably will not be two rectangles as shown -  I often find it easier to build up a shape from parts.

2) I used to "lock" sketches as has been indicated on this forum. However I seem to have problems moving the resulting solids as a result. They tend to "Stick". Moving components and bodies is, in general, is somewhat spotty for me-I was told somewhere not to use the "move" command and to be honest it is cumbersome when I just want to shift parts about on the screen. Sometimes components will move--sometime not--and I think it ties to locking their sketches.

  There is a whole area of moving parts, basic sketching, constraints, etc that is not well documented (hopefully in PDF) by the product- I find my self using lots of timely trial and error to guess how things work. 

Thanks!

Fritz

[TrippyLighting]

When creating the hole (This cannot be edited afterwards, I believe) you need to pick this option.

That will allow you to select sketch points:

I am assuming you're aware of it, but your sketches are not fully constrained.

[TheCADWhisperer]

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@fsonnichsen wrote:

not well documented

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>>Fusion 360 Documents<<

[fsonnichsen]

Peter-I have seen this in the forum somewhere, but it seems that I am able to pick up the "point" with the first option. Maybe it changed? Or beginners luck 😄

thanks

fritz

[fsonnichsen]

Yes-I bought a couple of these books a while back-- I think the first 3. A lot of good stuff and I refer to them on occasion--they are "example oriented" which was great for a beginner--but now when I need to look up a specific issue they are not usually specific enough- I always go to the Fusion doc side first but some of it is very precursory. I know this stuff isn't trivial and it just can't all get into one book!

IF you are allowed to-I would be interested in which of these books you like.  I guess I want something more "task" oriented--giving the specifics and "gottchas" of given tasks--a bit difficult to tell from the index

cheers

fs

[TrippyLighting]

With the single-hole option you can pick or really snap to a point, but that snapping will only be ate the time of creation of the hole. It is not parametric.

With the option I pointed out the hole will remain located at the picked sketch point even when the location of that point is changed.  

[fsonnichsen]

Ha! I never would have guessed----it is subtle--thanks for the advice.

Fritz

[HughesTooling]

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@fsonnichsen wrote:

Ha! I never would have guessed----it is subtle--thanks for the advice.

Fritz

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Have you seen the Fusion documentation, here for the hole dialog for example.

Mark

[fsonnichsen]

Sure Mark!

    I always go to the doc first (when there is some). I am glad you pointed this out because I think there are issues with the documentation. Documentation is not trivial with a product like a CAD and deserves a lot of attention when the code is written because that is where the subtleties appear.

    But the documentation for Fusion is often terse. A good example is what Peter pointed out concerning selection of a Point vs a Multiple Point Sketch. This may be somehow buried in the wording but it is subtle and important and I think it is worth a little deliberation. The writers of the code understood how it worked but past that things like this can get lost.

I think my biggest problem at the beginning of all this-was that I was "moving" the hole onto the Point using my cursor--and it never snapped. I finally found that I have to snap that Point--and not move to it--to get this two work. That is a little contrary to the "mouse culture" and not typical from my experience--so at least is should be mentioned.

    Another issue is that the Point on a sketch does not permeate the whole body-it only exists on the side were the sketch is placed. Fair enough--but good documentation addresses the major traps that a user might fall into before they happen-makes the forums a lot smaller! 

    And then there is the issue with Construction points at the Design (not the sketch) level. Apparently they don't serve as point locators for holes--seems like an odd omission-but if that is how it is-then it is worth saying that in good doc.

Take a look at the attachment-how would one place a hole at a sketch (not the Design Construction) point? The only point that appears to work--and only when the hole is moved about which is a bit subtle- is some type of "center point". Not sure what center this is-probably the CG of the body.

  If you search about enough you can accidently land upon this doc:

https://knowledge.autodesk.com/support/fusion-360/troubleshooting/caas/sfdcarticles/sfdcarticles/How...

OK-fair enough (if you were lucky enough to land on this paragraph). But try to use the sketch point to place the hole as mentioned and it does not seem to work. If you select "single point"--nothing happens-the  Sketch point is invisible. OK. Now- If you select "from sketch" things look good--until you snap the point--then you get "No target body found to cut or intersects". The point that is snapped is clearly on top of the target body--so it is not clear what went wrong. And---I still don't see how to get the hold on the point.

   All told Fusion is a good product and a lot of thought went into it-but like a lot of products in recent years the documentation could be more elaborative-A perusal of the forums is often a good hint as to how good the doc is. (Apparently there are AI routines out there that can scan forums to locate problems areas!)

Thanks Mark

Fritz

[HughesTooling · Accepted solution]

The error you see is because of the sketch direction (+Z-Z). Sometimes the Z points away from the body and you need to flip the direction. This is also why you can't use a construction point as it has no direction at all.

[fsonnichsen]

Crikey! Thanks Mark-that nailed it. 

   Honestly I did not realize that the "flip" icon was selectable-If I squinted enough I thought it was just a representation of the extent field. (Why didn't they make this an additional and more obvious field--it is important enough after all).  And since I am using the "ALL" extent I would assume that it goes in both directions through all of space.

    So I (and I think others) totally missed this. There is a very terse reference in the doc but with little deliberation I had assumed this only dealt with the position of which end the "head" might appear.

  I think if I read the doc like a lawyer might (I am NOT one!) I could have come to this conclusion-but again a little deliberation here (and perhaps more consistency in use of fields) goes a long way to make things self evident. (I see in the forums where others have had this problem).

  So I now have about 4 lines of notes that sums this whole post up-a lot with a little--a shame that the vendor does not do this.

Thanks all for your help-I think I have enough now to more forward with holes in the future

Fritz