When scaling a body, units are possibly preserved from pre-scaled body

[bbopp.apmachine]

I have a model body opened from (I believe) Solidworks that was in inches.

I scaled the body x 1/25.4 which provides a body that is in metric and appropriately sized.

Changing the size of a Hole that is 6.5mm diameter is incorrect.  Selecting the hole and pressing Q, the radius is display correctly as 3.25mm.

Changing the hole to 6.6 diameter by changing the radius to 3.30 (.05mm larger) creates a hole that is 6.5039 diameter.

Multiplying .05 x 25.4 = 1.27  --If instead of adding .05 to the hole radius, you add 1.27 to the hole radius (3.25+1.27= 4.52 supposedly mm) the resulting hole size is 6.6 diameter.

Somewhere in the calculation the base scaling is being maintained.

Very misleading as to what is expected of the user here.  Knowing the units previously scaled by is required + the knowledge of what the underlying software is doing which I'm personally unaware of.

In any case, unexpected behavior.

[TheCADWhisperer]

Can you File>Export your *.f3d file to your local drive and then Attach it here to a Reply?

Fusion is units “aware” - this should not be an issue.

In fact, I don’t even follow your problem description, hence the request for the file. This should all be automatic.  Can you post image of your current document units?

[jeff_strater]

@bbopp.apmachine - we will need a lot more information to help.  Ideally, as @TheCADWhisperer says - share the design itself.  Even before that, though, there are some questions:

• By default, a translated Solidworks design will produce a Direct Modeling design (no timeline).  Did you turn the timeline on after translation?
• "Changing the hole to 6.6 diameter by changing the radius to 3.30".  How did you make this change?  Did you use Press/Pull (or Offset Faces) in the Direct Modeling environment, or did you use some other method?

and a couple of comments:

• The body scale operation is ignorant of units.  It is just a way to scale a body by a given amount.  The fact that you scaled by 1/25.4 does not change the native units of the design.  You will have to do that separately.  (side note:  I am surprised that this scale is necessary - I was under the impression that the correct units and size should come over from a Solidworks import)
• If you do have history enabled, remember that Scale is an entry in the timeline.  If, somehow, the hole exists as a feature before the scale, editing that feature will take place prior to the scale, which also might affect things.

There well could be an issue here, but without more information, any way to fix or work around it will just be a guess

[bbopp.apmachine]

Capture Design History was enabled prior to alterations.

I've tried Q to push/pull alter size on Flat surfaces and that functions correctly but it does not on holes.

For instance:

You want to alter a hole size from 6.00 to 6.012 

This normally involves selecting the hole and changing it from 3.0R to 3.006R or by adding/subtracting the difference.

(A side note here:  This behavior is not always consistent --sometimes you put in the entire radius, other times/models only the change + or - is needed.)

In this file where the initial model was in Inches and scaled by 1/25.4 to get metric

You have to multiply the .006 * 25.4 to get a value that changes the hole to the correct size.

AFAIK this only applies to holes/cylinder because the metric value is correctly used on flat surfaces that are push/pulled.

[jeff_strater · Accepted solution]

Thanks, @bbopp.apmachine - it took a lot of head-scratching, but I understand what is going on now.  It is the "Automatic" mode for Press/Pull (or, more accurately, the "Edit Existing Feature" mode.  All Automatic does is choose between "Edit" and "New Offset").

I will say up front:  I hate Press/Pull.  If it were up to me, I would pull it completely out of the product.  All Press/Pull does is choose between other, existing commands.  Select an edge, Press/Pull invokes Fillet.  Select a profile, Press/Pull invokes Extrude.  And, the "Edit Existing Feature/Automatic" mode is, IMO, the worst part of Press/Pull.  This thread is a prime example of that.  What "Edit Existing Feature" does, for a face selection is:  try to move that face by editing the feature that produced that face.  For example:  If you use Extrude on a rectangle, you have 4 lateral faces, and one end face.  If you do Press/Pull on the end face of an extrude, in "Edit Existing Feature" mode, it will edit the Extrude depth.  If you choose one of the lateral faces, it will actually edit the sketch rectangle, and move that line that is driving the lateral face.  It was a nice idea, but just causes too much confusion, IMO.

OK, so, how does that explain what is happening here?  In the case of an imported design, the "feature" here is the Base Body Feature:

And, if you notice, this feature comes before the scale body feature.  So, this adjustment to the cylinder happens before the scale, which accounts for the difference you see.

However, if you use "New Offset" mode for Press/Pull, you will see that this gives the expected result - .006 offset gives a new hole diameter of 6.012.  That is because the modification is added to the end of the timeline (after the scale).

Or, you can use the Offset Faces command directly (my preference), and get the same result:

[bbopp.apmachine · Accepted solution]

Much appreciated!

Thanks.

[chuckA8JD8]

That is so helpful. I always used press/pull to "push" a sketch through a body and never thought of it for the fillet option but often use fillet. Thanks for the enlightenment!