In sketch, best way to place regularly-positioned corner holes?

[graham.wideman]

I often have a rectangular component with holes [Edit: Or posts, or square features or whatever] that are consistently positioned relative to the corners. What's the best way to set the position and diameter of just one circle, and have the other three follow the same size and positioning relative to the other corners?

Example starting point:

Desired result (or similar):

[Edit: To be clear, I don't want literally this result sketch with all the duplicate dimensions. The point of my post is to elicit best ideas on how to avoid the duplicate dimensions. The dimensions are just there to indicate the pattern of positions of the circles relative to the corners.]

I am aware of various methods that work but have shortcomings:

1. Most laborious: place 4 separate circles each with 2 distance dimensions plus diameter, with those three numbers controlled by parameters for consistency. Or...
2. Place vertical and horizontal construction lines across the vertical and horizontal center lines of the rectangle, then use "Mirror" twice to get the initial circle to the other three corners.  But that's quite a lot of steps and leaves a lot of distracting lines and symbols on the sketch.  Or...
3. Use a rectangular 2 x 2 pattern. But there the dimensions in the pattern are independent of the desired 7 x 5mm offset-from-corner, and would be wrong if I later resize the rectangle. That could be made more robust with a parameter or two. But seems like heading a little into the weeds.  Or...
4. Place a construction rectangle (or 4 construction lines) inside the original rectangle, and use its corners(/intersections) to constrain 4 separate circles. The construction rectangle could be created using the Offset tool, but only if the hole offset-from-corner is equal in both directions. The 4 separate circles would need a diameter parameter to ensure they all have the same diameter if later edited.

All of these methods seem more tedious than necessary for such a common operation.  I think the operation I probably want is something like "2-axis mirror", or "pattern relative to some other geometry", but haven't seen such.

Have I missed some clever way to do this?  Thanks!

[Edit: Apparently by initially mentioning "holes" as the features in the corner, the first respondents to this question wanted to lead me in the direction of the hole tool, which of course is not in the sketch environment. I have thus edited this to try and focus it on techniques in the sketch environment to position features near corner that might or might not be holes. However, I am increasingly sure that this is moot, as there does not appear to be a better way to do this within the sketch environment.]

[davebYYPCU]

Use the hole tool on the four construction corners, your version 4. (gives drilled tapped counterbores / countersinks in one step)

Use Constrains to have the holes symmetric of datum,

One of many ways to do it as you say.

Might help....

[graham.wideman]

@davebYYPCU  Thanks for your reply.

I'm not clear whether you're suggesting something specific with "Use Constrains to have the holes symmetric of datum,".  

It seems your recommendation mostly concerns whether to use a circle on the sketch versus the hole tool for the hole, right? Am I right that it doesn't cut down on the steps for size and position, and just uses one of the suggestions I listed?

For what it's worth, I often don't need the extra features of the hole tool, though if I did, then obviously it's a neater solution. 

[davebYYPCU]

Sounded to me that you were not mentioning symmetry when deciding how to space circles or holes, and you had already used the symmetry in the example sketch without mentioning it.

Not the hole tool - then you need the total number of circles and equals constraint.

Might help....

[graham.wideman]

> "not mentioning symmetry when deciding how to space circles or holes"

I thought I covered that in "set the position and diameter of just one circle, and have the other three follow the same size and positioning relative to the other corners?"

> you had already used the symmetry in the example sketch without mentioning it.

I labeled the example as "Example starting point" to convey that this is before adding the other three circles, awaiting application of some method to add and position those circles.

By the way, I forgot to note previously that one merit of the hole tool (as you suggested) is that it allows specifying in one place the diameter of the complete set of four holes, so that's a plus. On the other hand, it omits the circles from the sketch, where sometimes you want the circles visible on the sketch in order to help position other features. 

That said, the main topic of my question is still about whether F360 has some clever way to handle features relative to four corners as easily as mirror deals with pairs of symmetrical features or pattern deals with an array of features spaced relative to each other.

[davebYYPCU]

There is no magic button, unless you script it in API.

Add 2 more points to my sketch.

Allows 8 holes symmetric spacings, without a pattern.  (three timeline icons)

So what can't you refer to in my sketch, for other things?

Might help...

[graham.wideman]

I feel like so far the discussion has run into some communication or language difficulty. I have edited the original post to add an image of the desired result, and make it clear that the addition of three holes leads to a total of four holes, illustrates that they are in the corners, and positioned uniformly relative to those corners.

I've now had separate discussions with a colleague who's more thoroughly versed in F360, and he opines that there is no feature I've overlooked that makes this task easier. (Or should I say: specifies the hole positions more economically.)

But anyone who does have a bright idea is welcome to chime in!

[davebYYPCU]

Only communication difficulty, is that you want a complicated sketch, and I don’t.

Can wait for the Whispers comment on your second pic.  He doesn’t use duplicate dimensions either.

We will both get the job done.

[graham.wideman]

> Only communication difficulty, is that you want a complicated sketch

I think it's fairly obvious that I'm not requesting suggestions on how to complicate the sketch.

At this point we seem to be talking past each other, so I suggest we give it a rest.

[TheCADWhisperer]

@graham.wideman 

You have already gone too far.

Q1. What is the acceptable tolerance for the 40mm dimension?

Q2. What is the acceptable tolerance for the 60mm dimension?

Q3. What is the functional purpose of the component.

Q4. Considering Q3 and Q 1&2 what process will be used to manufacture these two geometric dimensions?

Mature MCAD apps like Autodesk Inventor Professional have built in tolerance specification/analysis, but in Fusion 360 we will have to consider our Tolerance Type (system) and Evaluate Size at +/- Median or Mean.

[graham.wideman]

@TheCADWhisperer  I appreciate you answering, but I'm struggling to see how your answer regarding tolerances and manufacturing has anything to do with my question.  I almost feel like you were answering some other post, except you mention 40mm and 60mm which happen to appear in my sketch.

My question is at the level of sketch geometry. Having positioned the first hole relative to its corner, i want the other three holes should be in the same spatial relationship to their respective corners. (Or some other method that positions all 4 holes at once with a single specification of X and Y offsets from the corner.)

I'm not seeing how tolerance comes into it.

[TheCADWhisperer]

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@graham.wideman wrote:

I'm not seeing how tolerance comes into it.

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I am leading you down a path to achieve an absolute answer that you cannot argue with - you will see the light at the end of the tunnel.

We cannot manufacture perfect parts in the real world.

Every dimension has an associated tolerance.

More specifically - I might ask, "What is the purpose of the 4 holes?" To fasten this component to another component?

Follow along and it will all make sense in the end.

What are your acceptable tolerances for these two dimensions?

[TrippyLighting]

Make a simple sketch:

Extrude to desired thickness:

Use hole feature and place with desired dimensions on corner:

Mirror hole feature:

Mirror hole and mirror feature:

Done!

My general advice:

Move past the sketch quickly and model in 3D features!

In more complex scenarios than a block, that is faster and less laborious than trying to constrain and debug complex sketches. It also creates computationally faster and more stable models.

[g-andresen]

Hi,

just try this

günther

[graham.wideman]

@TheCADWhisperer 

I still don't know where you're going with this.

But for the sake of argument, let's say the outer rectangle is the perimeter of a PC board that I need a model of (for which I don't have CAD).  Say I'm good with +/-0.2mm on the sides. Or likely the actual boards have more variation than that (due to edge snapping), but the holes are consistently placed within the original design coordinate system that had a well-defined edge rectangle.

The near-to-corner features might be to create a hole, or could be two concentric circles that would go on to extrude to create a cylindrical standoff to include in the model, with a hole in the middle.

This example I just contrived here would produce a model of an object to use in F360, and does not go on downstream to a manufacturing process.  I could contrive an example that would be used for a 3D printed or milled aluminum object, but at the moment I don't know where you're going with all this tolerance discussion.

[graham.wideman]

@TrippyLighting  I appreciate the effort you went to to create that example.

I think your point is: if the feature is a hole, use the hole tool.  Yes, I know that.

But my question was really about geometry techniques in the sketch environment. Apparently I distracted you and others by using "hole" as the example corner-relative feature.

One relevant point I did glean from your answer was using Mirror twice to replicate a defined-once feature to the other three corners. Which was one of the techniques I listed in my original post. So you're probably confirming that F360 doesn't have some clever 2-axis mirror operation.

[graham.wideman]

@g-andresen 

Though you didn't show it, I infer that before the beginning of the video, you set up a 2x2 pattern of circles or holes, with the pattern parameters for shape spacing calculated from formulas based on rectangle width and height.

So that requires five parameters to control the first hole, and two more to calculate the X and Y spacing. (Strictly speaking, I guess we don't need the diameter to be a parameter.) 

I like that it does keep the sketch tidy, at some expense of cluttering the Parameters list, and a bunch of typing.  Not exactly the "shortcut" I imagined, but sheds some useful light on this task. Thanks!

[TheCADWhisperer]

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@graham.wideman wrote:

@TheCADWhisperer 

I still don't know where you're going with this.

 Say I'm good with +/-0.2mm on the sides. 

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OK, that is just the board size tolerances.

We also have two position tolerances and one size tolerances for each hole.

You asked about best technique - before we discuss that  - note that there are eleven different Tolerance Types (strategies) without even taking into account GD&T (Geometric Dimensioning and Tolerancing).

I didn't ask you about tolerances for positions of the holes, but I will assign +- 0.1 for discussion.

Let's examine these two holes as you have dimensioned them.

Nominal distance between holes is 46mm.

Fact 1. At upper limit of the 60mm the width of the board is now 60+0.2= 60.2mm.

Fact 2. At lower limit of the horizontal position of the left side hole it is now 7-0.1=6.9mm from the edge as dimensioned.

Fact 3. At lower limit of the horizontal position of the right side hole it is now 7-0.1=6.9mm from the edge as dimensioned.

Fact 4. The distance between centers of these two holes is now 46.4mm rather than the nominal 46mm.

These are facts.  Simple Addition and Subtraction.  And this is only one possible combination of 3 of the dimensions.

@graham.wideman 

You asked about the best technique.

Q. Does the scheme we choose directly effects the final geometry? (Multiple schemes have been suggested in this discussion thread without any consideration of effect on function of the component considering real world manufacturing tolerances.)

The clever way is to first consider the function of the geometry. (Any geometry - holes or other.)

It isn't just about making work easy/fast.  It is about doing things that work (in the real world).

(See first two SpaceX Starship heavy boost rocket launches for examples of not doing things that work in the real world.)

Using your actual example - if the critical factor is the distance between holes - then there are better techniques.

[TrippyLighting]

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@graham.wideman wrote:

@TrippyLighting  I appreciate the effort you went to to create that example.

I think your point is: if the feature is a hole, use the hole tool. 

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No, that is NOT my point. My point is. that you need to move away from sketch based geometry into 3D features as soon as possible.

The purpose of a sketch in a parametric CAD modeler is to provide as simple as possible base geometry for extrusions, revolves etc. The rest is to be modeled using 3D modeling features. This isn't a "hard rule" but more of a guideline.

For example, I almost never mirror in a sketch or create a pattern in a sketch. I avoid construction geometry and work with constraints to keep sketches uncluttered and the design intent recognizable on first sight. Sometimes this is more up-front work, but tremendously helps as designs progress through many iterations. over time.. 

This advice is based on 30 years of professional CAD use as an Engineer with well over 20 of those in 3D starting with (but not limited to) SolidWorks in 1998!

[graham.wideman]

@TheCADWhisperer 

OK, you've recounted some basics of dimensional error or tolerance stacking.

How does that apply to the sketch environment? I have not encountered a feature set in the sketch environment to capture tolerances -- have I missed something?

I'm pretty sure you're not referring to stacking of tiny errors in F360's dimensional precision are you? (Apparently that's 6 digits, so I'm not too worried about that.)