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Drawing Dimensions are Incorrect

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Message 1 of 51
bkisker
9130 Views, 50 Replies

Drawing Dimensions are Incorrect

Hi,

 

I'm missing something obvious here and cannot figure out what it is. Video is embedded to demonstrate what I'm seeing (you'll want to view full screen so you can read dimensions). 

 

I'm making a simple cube with units of inches. When I create a new drawing from design, the automatic dimensions (also in inches) do not match.

 

 

I'd appreciate any help! 

 

Thanks,

 

Brett

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Message 2 of 51
cmiller66
in reply to: bkisker

Hi Brett,

What you're showing is not supported (yet) in Fusion drawings.  The dimension you're getting in the drawing is the 2D projected distance of those 2 points, not the 3D distance.  It looks like we do have a bug here though. If you place a base view with orientation NE Isometric (or any of the isometric views) you'll get a tooltip that you can't place dimensions to the isometric view.  We should be blocking dimension creation and displaying the same tooltip for Home orientation too.

 

We do have support for dimensions to isometric views on our roadmap.  Currently though, you'll need to dimension the Ortho views.

 

Thanks,
Chris

Message 3 of 51
hhelmbold
in reply to: cmiller66

Hi - I don't understand what you mean this is not supported? I find this absolutely unacceptable unless I read it totally wrong. You telling me if I design a part and want to give someone a drawing to make the part it cannot be done because the dimensions will be completely wrong?

 

I created just a basic tower with a base of 35mm - bringing into the drawing at a 1:1 scale suddenly makes it 29mm?? This is a serious bug.

Message 4 of 51
cmiller66
in reply to: hhelmbold

Hi hhelmbold,

Currently, placing dimensions to Isometric views in a drawing is not supported.  If you select the Dimension tool and try to dimension to this view you will see a message:

ISO_dim.png

The individual dimension tools in the drop-down menu still allow points on these views to be selected. This is actually the bug, until we support dimensions to iso views we should be blocking this.

 

Dimensions to Orthographic views (Top, Front, Side, etc.) are supported.  A base view of your design with orientation Right, or Front will dimension correctly to 35.00.  The distance you are dimensioning needs to be orthogonal to the sheet, otherwise the value is the 2D projection of that distance, not the actual 3D distance.

 

For angled faces you can place a base view with a custom, named view orientation.  In the design select "Look at" at the bottom of the app window, select the face, and then right-click Named Views in the browser and save this view.  In the drawing you can then select this as the orientation for your base view.

 

I will re-forward the request to support this to the team.

 

Thanks,
Chris

 

Message 5 of 51
hhelmbold
in reply to: cmiller66

Thanks Chris, your reply means a lot. I understand now what you mean with "it's not supported" - I just needed a 3D sketch to scale without all the other views. I will appreciate it if it can be forwarded to the support and development team. This is something that should be supported... It is very time consuming going through all the other views and making sectional drawing just to get to scale 3D drawing for printing.

Message 6 of 51

@cmiller66  It is now 2 years after the initial report of this embarrassing bug.

 

It hasn't changed. You are still unable to display a dimension of any part in a 3d view!

This is a poor, very poor lack of a simple function that makes drawings almost useless and a burden to work with!

 

It is August 2020 and you haven't bothered to implement this very basic function? What hinders you from doing so?

The design workspace can already do any measurement, in any view, why can't the same program use the exact same code to measure a drawing view? It's referencing the same bodies, edges, etc..why does it "NOT SUPPORT" doing the exact same task it can do everywhere else in the program?

 

That's like going to a store and asking for 10 apples, and they give them to you.

But then you ask for 10 oranges and you get 7 and 1/3 oranges because counting oranges is not supported?

What the ****.

 

What kind of programmers achieve such an incompetent mess, but also were able to code other, way more complex functions without problems?

 

This is very, VERY weird.

 

Please explain!

 

@Alfred.DeFlaminis, maybe you can help here?

Message 7 of 51


@Evil.Kitten.Studios wrote:

That's like going to a store and asking for 10 apples, and they give them to you.

But then you ask for 10 oranges and you get 7 and 1/3 oranges because counting oranges is not supported?


I think it would be more like Apple coming out with a new iPhone that doesn't have all of the functionality of the current iPhone... ...plus a bit more.


You can do True Dimension (or Projected Dimension) in Autodesk Inventor Professional 2D drawing environment.

AFAIK, you could do this 2+ yrs ago... (actually I think much more than 2 years ago, but my memory isn't what it used to be).

 

Message 8 of 51

Hi @TheCADWhisperer , @Evil.Kitten.Studios  - 

Drawings Product Manager here - I wanted to chime in since this thread has been revived. We don't have dimensions for isometric views on our road map for this year, but we hear it from customers very often, recognize the need for it, and hope to get to it once we've delivered additional highly-sought after view types and other missing functionality such as hole & thread notes, weld symbols, and all-level parts lists. While I understand the surprise that this functionality is missing, since Inventor supports it, iso dimensioning is a limitation in AutoCAD, which provides much of our back end architecture. Thus, supporting it isn't as simple as it might seem, and we need to balance prioritization of this project with the other big-hitters on our backlog.

 

In the meantime though, I agree that we should be more consistent with the tool tips and locking of dimensioning  for these types of views - we're discussing how we can make this experience better until we can deliver against the underlying need. Thanks for raising this again and for the continued feedback as we work to level-up Drawings in Fusion 360.

Message 9 of 51

@olivia.struckman Thanks for the insight. Does your title mean you are only in charge of the drawing workspace in fusion?

 

However:

"iso dimensioning is a limitation in AutoCAD, which provides much of our back end architecture."

 

Again, Fusion (and AutoCAD of course) can already measure and dimension objects in the design workspace in both perspective and ortho views.

So then why does it do the same task different and wrong, just because you chose a different visual projection?

 

 

" Thus, supporting it isn't as simple as it might seem"

 

..but it seems really, really simple.

In a drawing you are always referencing existing bodies from a design in fusion.

Simply stated, a fusion drawing takes pictures from different angles of things you already made and lets you place and arrage them as you wish on a sheet of paper.

 

So why, please god why, is it so hard to get the values of the edge, area, etc. measurements into a isometric view?

 

The parts never change. The dimensions never change. Only the visual representation of the scene changes.

Why is is not possible to achive such a simple, basic function? It's a matter of storing numbers in memory or even the save file, which obviously they already are stored in, and retrieving those numbers.

 

That's like asking a friend to measure your height with a tape measure and he tells you a number.

Then you turn to your right and ask him to close one eye and measure again and he says: "This is impossible. I can only do that with both eyes open and you facing me. Maybe next year."

 

Who comes up with those decisions to take something that works in the same program already and make it not work in one specific instance?

 

I would greatly appreciate a peak behind the development curtain here.

I am a hobby game developer myself and things like this rob me of my sleep sometimes.

Thanks

Message 10 of 51

While the modeling environment is aware of the actual 3D dimensions, the 2D drawing space is not.  The dimensions created in drawings don't have pre-canned values based on the points or edges selected, they're generated at the time of creation to reflect the paperspace distance selected with the scale of the view taken into consideration.  The dimension value is  a 2D projected distance of that edge/points. Thus, supporting this requires some fundamental rework on our end (just as supporting MBD would), and it is a big project. I wish it were simple, trust me 🙂 

Message 11 of 51

"The dimensions created in drawings don't have pre-canned values based on the points or edges selected, they're generated at the time of creation to reflect the paperspace distance selected with the scale of the view taken into consideration. "

 

Forgive me for saying this, but that idea still makes no sense to me.

 

The dimensions are generated to reflect the paperspace distance at the selected scale.

 

The paper is a 2D environment with a fixed size (like A4 with 210x297mm).

You want the drawing to show a product (let's say a wooden sign) that has the dimensions 1000x500x100mm.

You insert the component into the drawing at scale 1:10 in a top down projection.

That would make it's dimensions 100x50mm on the paper. That would fit nicely.

You put that view to the top right of the paper.

You also want a nicer image for the costumer, so you also insert the standard NE iso view.

You choose a bigger scale and a rendering type that shows the texture so there is more to fill the page.

You add dimensions to the top view. They say 1000x500mm.

 

Now you add dimensions to the 3D view.

They are now something arbitrary, because they are actually measured in "paperspace".

They neither reflect the actual component, nor do they provide any help to anyone else who would read the drawing.

Instead it creates confusion over which dimensions are meant to be correct. Or if there are two different parts shown.

 

All the math the drawing workspace should do with a component is to scale it according to the paper size, taking the real units and dividing them by whatever scale the user wishes.

 

A part that is 800mm long in reality, should be exactly 100mm long on a 1:8 drawing.

The marked dimensions should always say "800mm".

Nothing more, nothing less.

And certainly not two different values, depending on which way you view it.

 

Nobody benefits from looking at a drawing of a 80cm part that is marked as 63.30860483cm, right?

 

Don't you agree?

 

"The dimension value is a 2D projected distance of that edge/points. Thus, supporting this requires some fundamental rework.."

 

The other projected views like top or right already measure the correct dimensions. I don't see the issue.

The drawing workspace already measures components correctly when they are viewed from any 2D side!

This is why I don't get how this should be any challenge at all.

 

Any component in the drawing file references a component in a design.

 

Take the wooden sign:

There is 1 component. Store an index as a short or whatever.

It has 8 points, 8 positions as 3D vectors.

It has 12 edges connecting those points. 12 floats for their length.

It has 6 sides. 6 floats for the area measurement for example.

 

Regardless of how these are handled internally, you already measure those values correctly in all 2D views inside the drawing.

And they don't change when working on the drawing.

They only change when the design, which they reference, changes. And that change is updated as easily as refreshing a web browser site.

They are the same in 2D as they are in 3D, just make the 3D view display the correct value which is already achieved in the 2D views and this problem would be solved.

 

Component 1 has edge 01 that is 10cm long. 10cm is the dimension. Across all views. Simple.

How big edge 01 is on the print, where it is positioned, or which way it points because of the view angle,

is irrelevant and purely a visual effect.

How you scale it, render it, name it, etc.. what does that have to do with any of the dimensions? Nothing.

 

Am I wrong?

 

Thanks.

Message 12 of 51
DavePlant
in reply to: bkisker

Hello, I just  came across this problem - where dimensions on ISO views are wrong. (They are actually projected 2D distances in paper space).

 

I would strongly suggest that Fusion 360 blocks the user from adding aligned dimensions to an iso view, if they are known to be wrong. It seems to block linear dimensions - wisely. The big risk here is the user adds them, trusts the software,  sends out the drawing. I understand it will take work to fix it. But at least disable aligned dimension being applied to ISO views until the functionality is added.

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Message 13 of 51
4sommer
in reply to: bkisker

What worries me the most is that this discussion started in 2018 - We now write 2021 and notthing have changed... is it really on the roadmap?

Message 14 of 51
g-andresen
in reply to: 4sommer

Hi,


@4sommer wrote:

.. is it really on the roadmap?


Roadmap

 

günther

Message 15 of 51
4sommer
in reply to: g-andresen

cool... it is on the roadmap😀

 

Let's hope this year will be the year we see this function then

Message 16 of 51
SheridanTech
in reply to: bkisker

Ok, so yay, it's on the road map...  but just how long is this road?   (Without dates, it seems more like a river?)

 

True Dimensions on 3D Views is a much needed feature but which most confusingly is currently 'partially but incorrectly supported'...    (e.g. Think about all those manuals with 3D views for end users etc etc!?!?)

 

The fact that F360 Models and Drawings are insufficiently connected* is a concern:  it seems that drawing views are just 'flat' projections to 2D 'paper-space'... so adding dimensions shows the size of the 2D drawing only (with scale taken into consideration).  Hence only edges/distances that are on the 2D view plane are true dimensions that match the 3D model.  Any edge at an angle to the 2D paper space (as in isometric views etc), is not a true length/dimension - its a projected (2D only) length/dimension.  And seemingly, there's no simple way to 'fetch' the true dimension?!

 

Let's not forget that some users will want to show a projected dimension on 3D views (though, I can't think of an example!?). Fusion needs both types implemented.

 

[*Solidworks has the option to switch between projected and true dimensions on any view type: but SW drawings are much more tightly linked to the model.... (a 2 way sync - to the extent that dimension changes in the drawing are reflected/synced back to the model).]

 

 

Message 17 of 51


@SheridanTech wrote:

[*Solidworks has the option to switch between projected and true dimensions on any view type: but SW drawings are much more tightly linked to the model.... (a 2 way sync - to the extent that dimension changes in the drawing are reflected/synced back to the model).]


Autodesk Inventor Professional has this functionality.

Message 18 of 51
phunk80
in reply to: bkisker

 

Hi guys,

 

I´d like to pick up the conversation here at this point to not open a new thread.
I designed a speaker with a 3 degree backwards tilt. Now I try to create the drawing for the carpenter but measurements in the drawings do not match. The actual size of the front edge of the part is 1040mm. The projected view shows 1038.57mm which is correct from a mathematically projected point of view but not the measurement of the actual part. 

What am I doing wrong here? 

Thank you

 

 

Screen Shot 2021-10-04 at 20.06.50.png

Message 19 of 51
SheridanTech
in reply to: phunk80


@phunk80 wrote:

...3 degree backwards tilt...measurements in the drawings do not match.... actual size...is 1040mm. The projected view shows 1038.57mm which is correct...

 


You are not doing anything wrong as such, and the drawing and dimensions are correct:  the 1038.57 is the vertical height of the front face (as projected on to the plane of the drawing).  

 

It's important to realise that Fusion can only display projected dimensions. So dimensions of model items on (or parallel to) the drawing plane (=sheet) will be true dimensions (e.g. the "1040" dimension). Model items that are not parallel to the drawing plane will give projected dimensions. (e.g. the edge dimensioned "1038.57").

 

So, the 1038.57 dimension is 'as expected', but it would be clearer to add this (as a vertical dimension) on the righthand view.   However, I would suggest removing the 1038.57 dimension altogether to avoid confusion and add the width dimension on the lefthand view (that edge is parallel to the drawing sheet/plane so will yield a true dimension). Only actual width and length are then displayed.

 

For the record, in Orthographic projections, all dimensions should be projected and would be read as such. So, if the 1038.57 dimension were 'forced' to show the true length of 1040, this would be non-standard & confusing.  This thread is requesting a 'show true dimension' feature primarily for use in '3D drawing views' (e.g. isometric) rather than flat 2D orthographic, projected views.

 

Additionally, in more complex cases, you could create an auxilliary view of the front face. This would give a square-on view of the object so that all edges - and therefore their dimensions - are actual/true.

 

Hopefully I've understood you correctly? 

 

Extra tip:

You can get a 3D 'picture' with true dimensions is Design mode, as follows:

  1. Add dimensions to sketches
  2. Show the sketches that are relevant
  3. Browser >> [right-click a sketch] >> Show Dimensions
  4. Rotate the view so the dimension text is clear
  5. Set opacity etc
  6. Screen shot it etc

 

It's crude, but it does allow screen-shots to be taken and used in documentation (and inserted in a Drawing… I think????).  However, it also demonstrates the need for true dimensions on 3D views in Drawings! 😞

 

Message 20 of 51
phunk80
in reply to: SheridanTech

Thank you very much for the explanation and your help!

That is a bummer. IMO this is a basic feature of a CAD App and very necessary when creating drawings for manufacturing. It is a massive amount of time to check every component in an assembly fo parallelism to the sketch plane. 

The auxiliary view tipp is golden, thx. The workaround with the sketch dimensions is nothing but ridiculous. We´re talking a grown up CAD systems here ...

 

As far as I researched yesterday night this is a requested feature for years, isnt it?

 

 

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