Trick to get units to change from in to mm?

[jdholbrook33]

Needed to make some fixtures for some new parts. Received a drawing that was in inches.

I changed the units (Document settings > Units) for the project to inches to simplify using the drawing.

After I completed the model I went to Document settings > Units and changed back to MM (default is checked for this)

During CAM I came across a few things that needed to be changed. When I went to Design and tried to change dimensions, they are shown in MM but when I try to change the value, the entry box is in inches. So it shows MM for the model dimensions but shows inches when trying to change dimensions.

How do I get this project to be pure MM ??

I mean shows MM and also accepts input in MM??

[seth.madore]

This is something I've noticed as well, and I suspect it's an annoying bug. One thing you can do when typing in dimensions is force the "MM" by using 1mm (as an example)

[jdholbrook33]

Annoying bug?

It gets worse.

I just now tried to modify the dimension, it shows 30.49mm on the dimension, when I click on it to change it shows 1.20 inches. I changed it to 1.40 and it accepted it as mm so now my circle is 1.4mm diameter. WTF???

that's much more than an annoying bug.

So when the input box shows "1.200 in" and I input 1.40 and hit enter I get a 1.4mm diameter circle is an annoying bug?

Completely forget the fact that 1.200" equals 30.480 mm. NOT 30.49.

It's an annoying bug until you ruin a part because you're trying to bore a precision hole. Spent 30 minutes or more calibrating my end mill, getting the TIR down to 0.0002". boring test holes to get the wear offset so a 20mm hole is 19.999mm

That is not an annoying bug, that is a major flaw.

Here's a hint: Stop adding new features and working on useless cosmetic upgrades and make the program actually work.

the number of "workarounds" is piling up and it's pretty high now.

[seth.madore]

I don't suppose you could share the file, even if only privately? I don't often deal in MM > IN conversions, so I only have passing experience with what's going wrong.

[TheCADWhisperer]

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@jdholbrook33 wrote:

I changed it to 1.40 and it accepted it as mm so now my circle is 1.4mm diameter. WTF???

 Type in 1.40in NOT 1.40 Fusion will automatically make the conversion for you.

I suspect that there is a far far easier solution though.

Can you Attach your file here for testing?

[jdholbrook33]

Here is the file.

If I type in 22.225mm then it is in mm the next time I open the dimension.

Some of them have been changed to mm this way already but there are plenty that are still in IN.

If I open a dimension and close it without making any changes, it remains in IN.

Just to note. I made this  yesterday and Fusion was closed and computer shut down over night.

Noticed the dimension issue this morning.

Thanks,

James

[jdholbrook33]

Tired of workarounds.

If I don't use them often they are forgotten and the next time.. I'm once again wasting time.

Time is money.

Money wasted because the software wasn't built correctly is ridiculous.

Especially when a lot of effort is being put into making new features (some of which don't even work).

/rant off

James

[TheCADWhisperer]

Each dimension has a name...

Some of the dimensions were originally created with inch units (as you know).

If you change any dimension - you should not see any issues if you type in the units.

For example if you want 1.4 inches - type in 1.4in.

If you want 100 mm - type in 100mm.

Now, because  your current document units is mm, you should not have to enter the units.

If you can demonstrate a way that a new dimension (or edited existing) dimension does not take on the current document units (mm) I would be interested in seeing a Screencast Recording of the steps.

Bottom line - if you type in the intended units (in or mm) you should never ever have an issue - even when working in a mixed unit environment.

[jdholbrook33]

If I select MM as the document default, why isn't everything converted to MM?

Other wise why even have document default?

When I set default to MM, I hope to see MM EVERYWHERE at ALL TIMES.

It's a programming error to still have IN even visible.

especially when I see 30.49 mm as the dimension but when I click it to change, it reverts to 1.200 in.

That leads me to believe it's still in IN so I enter the value in IN and viola.. it's not in IN anymore it's MM now??

You can't deny that is a bug.

If I have default set to MM and I want to enter IN, I'll enter it as 1.200 in, that's logical.

Setting default to MM and having to enter 30.48 mm is not logical.

How do you explain me getting 30.49 when the measurement should be 30.48. 1.2000 inches is 30.4800 mm.. NOT 30.4900.

Somebody screwed up somewhere.

I am not installing Screencast to illustrate the problem when it is plainly visible right there in your screenshot and the two I sent before.

In your screenshot there are IN and MM values.

Why aren't they all MM if I change "default document units" to MM??

Some distorted logic there.

[TheCADWhisperer]

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@jdholbrook33 wrote:

1. You can't deny that is a bug.

2. How do you explain me getting 30.49 when the measurement should be 30.48. 1.2000 inches is 30.4800 mm.. NOT 30.4900.

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1. I have been working in a mixed unit environment for more than 40 years, first out on the shop floor and later on computer.  It all looks perfectly logical to me.

2. I looked over your model twice and I do not see this anywhere in your design.  Can you post screen shot pointing it out (sometimes it is easy to miss the obvious)?

This can all be explained logically, but might take a few attempts.

BTW - MM is not a valid unit in Fusion.  It must be lowercase mm.

[TheCADWhisperer]

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@jdholbrook33 wrote:

How do you explain me getting 30.49 …

I am not installing Screencast to illustrate the problem…

Some distorted logic there.

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Even though you are not willing to create a video for your issue,  I am ready and wiling to take  the time to create a video explaining the logic (which is the same logic used by Inventor, SolidWorks and Creo). It will all make logical sense.

But first I would like to know where/how you are seeing that 30.49 dimension (or measurement) as I can’t find it.

[jdholbrook33]

You're right, I'm wrong.

[CGBenner]

@jdholbrook33 

Are you still having trouble with this?  At any point did you switch the active units from in to mm, or vice versa, after some features had already been modeled?

[jdholbrook33]

Hi,

Thanks for asking.

My default unit for Fusion is millimeters.

I started the model in millimeters since I had used my mill to precisely measure my stock and my mill is set to millimeters. I modeled my stock in millimeters then considered doing hand calculations to change the part from inches to millimeters. I though it would be easier to model the part in inches since the drawing was in inches. Once I had the part modeled, I switched back to millimeters and proceeded to make the modifications to the part that I needed.

The first modification I wanted to make was to change the 1.2" pocket to 1.4". The first thing I noticed was the 30.49mm measurement which should have been 30.48mm. I called my head machinist in and showed him. I switched back and forth from "selected" to "un-selected" to see the 1.200" change to 30.49mm.

I had seem some weirdness in the past with such behavior and it turned out the number was being stored as something like 1.2000993" and the software was rounding up when doing the conversion.

I saw 1.200" in the input box so figured I needed to input 1.400 to change it to the number I wanted. I typed in 1.400  and hit enter resulting in a pocket that was 1.4mm in diameter.

I did a quick calculation and entered the value in metric for 1.400" (35.56mm). So the 30.49mm was lost.

If I open the part, activate and edit the sketch (second sketch in the list) I see all measurements in millimeters but when I select a measurement, I see the measurement in inches.

Is that the  way the software should operate?

Why not convert everything to millimeters?

It could get very confusing when you're expecting the measurements to all be in millimeters.

Thanks,

James

[HughesTooling]

Try this simple test. What I did was start by dimensioning one side with the document set to mm (set size to 25.4) then change document to Inches and dimension the other length to 1. Now if you look in the parameters dialog you'll see the expression is what you typed in using the document units at that time. Changing the document units does not change what you typed in (don't forget the expression might be more then just a simple number). When you change the document units all that changes is the VALUE for the model parameters, this is what you see in the sketch until you try editing it then you see the Expression.

For the inaccuracy you had for the 1.2in size, did you use grid snaps or did you actually type in 1.2? I've seen inaccuracies like this if you use grid snaps or just drag to a size, I've found typed in sizes are always accurate. Not sure you really need to change the document units if you just need to dimension a couple of sizes as it's just as easy to type in the size with it's units, 1.2in for example might be an easier workflow. And as said before this is all pretty much standard for how parametric modelling programs work.

Mark

[TheCADWhisperer]

I will create a video when I get a chance - but in general, it is desirable to preserve history of dimensions (just like history of features).  That is perhaps the most powerful foundation of parametric history-based modelers.

In a mixed unit environment in the conversion you will end up with numbers that appear to be very "odd".

We can interrogate the history/parameters and see, "Ah, now that makes sense as a conversion of a "normal" inch dimension to millimeters or a normal millimeter dimension to inches."

This could be a "chain of evidence" down the road, "Where did this number come from?"  If we destroy the evidence, we break the chain.

We used to have to remember conversion factors.  If we mess up, well we crash multi-million dollar spacecraft into Mars.  Now it is simple, no conversion necessary - simply type in your intended units and the software will take care of the conversion for you.  (And keep a record of it so that next year, month, week, tomorrow - someone else can see how you came up with that number.) 

I often see models where none of the sketch dimensions make logical "sense" (or missing dimensions altogether).

First thing I do is check in dual units all decimal places.  They will make "sense" in one unit or another or I then assume the designer did not really know what they wanted (or how to get there).

[jdholbrook33]

Just seems to me it would be a lot less confusing where if I selected Millimeters, everything is in Millimeters.

EVERYTHING.