Drawing thinks base view is an isometric projected view??

[rklopp]

I am trying to make a drawing from a component. I lay down the base view and then project orthogonal views from it. When I go to dimension things, the tool shows a circle/slash and says I cannot dimension isometric projected views. I don't have any isometric projected views. I even started over and laid down a new base view and deleted all the other views, and still get the same error. I also cannot make center marks on circular features, and the diameter dimensioning tool refuses to recognize known circular features. This has happened since I installed the 12/16 update this morning. I made sure my 3D component is aligned with the coordinate system.

Any ideas?

[cmiller66]

Hi rklopp,

Sorry to hear you're having an issue with drawings.  We didn't have any drawings-related changes in the last release so I'm surprised to hear this problem is new.  Can you share your design or project with me, christopher dot miller at autodesk dot com so I can take a look?

In the design do you have any named views, or possibly reset views (from the drop-down next to the view cube in the design)?  If you try with the simplest case, a cylinder drawn on the default plane in a new design does that work?  It should make no difference but are you on Mac or Windows?

The single dimension tools (these are available in the drop-down on the Annotation toolbar) should still work as expected.

Thanks,
Chris

[HughesTooling · Accepted solution]

I guess you're using a named view like I suggested in your other thread. I've done this before and had no problems applying dimensions, just tried again and saw the same problem you were seeing. After reading what Chris said about using the single dimension tools it all works how I remembered. So the key is don't use the multi dimension tool with a named view as the base view in a drawing..

Mark

[cmiller66]

Hi Mark,

Thanks for the post.  Just an FYI, we have a defect logged in the system to further investigate this - provided the named view is truly orthographic the dimension tools should still work as expected. The reason we block the single dim tool for isometric is because the dimension value will be for 2D projected distance in the view, not the actual 3D distance in the design.  We plan on offering auxiliary views in the future (not sure where this is in the roadmap, but not in an immediate update) which should address some of these issues.  Thanks for your patience.

Thanks,
Chris

[rklopp]

Thank you. I was wondering what that funny array of yellows arrows was that suddenly showed up on my dimensioning tool! I must have accidentally picked it and got it into the toolbar. Oddly, when I searched "multi dimension" in Help, nothing came up. Now the dimensioning tools except for the center marks seem to work.

[Maowen_Zhang]

@rklopp, Mike, as Chris mentioned, we tracked one similar issue in our internal system, I checked it and found a proper solution to fix it. 

But we haven't found how the issue generated, and not sure whether it could fix your case, could you provide some details about how to reproduce it from scrach, how do you use named view / set current view as Front (select a face that not exactly orthogonal)? It would be also help if you could share a design (you could delete unrelated contents in f3d if need) that has this issue with us. Thank you! 

[HughesTooling]

Hi Lori

Here an example test file using a named view. The multi dimension tool doesn't work on any of the features.

The single dimension tools work fine.

Files Attached. Why can't I attach f3z files?

Mark

[rklopp]

The dimensioning seems to work fine if I export the component of interest as an archive,  re-import it into a separate project, rotate the component back to the orientation of the base sketch, and then make a drawing. The trouble seems to be that the component is no longer aligned with the base sketch. This may be because I moved and roatated the component when making a joint with another.

[rklopp]

Attached is a test case. By making the flat face of the square the Top even though it originally was at an odball angle, I am able to dimension the diameter of the circular part in a drawing. However, center marks fail to stick. Is there a way to export a drawing in the native format? I only see Output DWG and PDF, and Export does nothing.

My difficulty lies with a much more elaborate assembly with lots of joints and rotations. The drawing tools seem to fail to recognize circles and arcs as such, even though the drawing projections are orthogonal to known flat, circular faces.

[HughesTooling]

Try using the dashbord to export the drawing file, you should get an fz3 file that contains the drawing and the 3d files used in the 2d drawing.

Mark

[rklopp]

My first question was WTH is the Dashboard? I  thought the Dashboard was the left panel in Fusion, but I could not find an Export command there. Searching "Dashboard" on the forum got me enough clues to figure it out, but there are times when a formal manual or help system would be helpful. I found that if I opened a webpage to A360, I could eventually export the drawing as an f3z file, but then it took a while to figure out that the exported file stayed in the cloud, which is not exactly exporting to my way of thinking. Is that what you meant by Dashboard?

In any event, I finally got a download of the misbehaving drawing file, and it is attached. <More frustration - I can't attach an f3z file to a post. Why not? See zipped folder.>

[kris_berg]

Hi @rklopp,

Sorry for the confusion.  The dashboard is the same thing as the "Data Panel" in the Fusion 360 help.  You are correct that export is not an option there. The way you exported the drawing (from A360) was correct.  Another alternative to share files is to use the "Share Public Link" command in the context menu for an item in the Data Panel.  This allows others to download the .f3z without you having to attach it.  

I am not sure why you cannot attach .f3z files to the forum.  I will see if we can get that fixed.

Thank you,

Kris Berg

Fusion 360 Development

[Maowen_Zhang]

@rklopp, thanks for sharing related files which are very helpful, I started checking this, but haven't finished yet, keep you updated!   

[rklopp]

Maowen,

Have you been able to invistigate the issue?

Thanks,

RKlopp

[Maowen_Zhang]

@rklopp, I did research on this but was interrupted by others and haven't found a fix solution for it yet. From the research, the drawing view's direction or body's face doesn't exactly match XYZ axis direction, there is 1.0-4 difference which lead to the extra arc and smart dimension treat it as ISO view incorrectly. I will back work on this tomorrow or Friday and update with you when it's resolved. Thanks a checking! 

[Maowen_Zhang]

@rklopp, I checked this issue today, it's related with tolerance of view direction, the view direction become lower 1.0e-5 when have some transforms (joints, rotation, etc.). I'm working on a fix which should be ready post January release.

In the meantime, one workaround to get correct drawing view resuts, add dimension and center mark is "from browser select component Crankshaft, save Copy As a new file, then create drawing from it". The result shows as below. It's just a workaround in case you need a drawing from it.  

  

This issue happens on this special component which has some joints (transforms on it) and get lower tolearnce issue that we need to fix. In this same file, other components should work fine.  

Such as below highlighted face, select it, look at it and set it as Top view, the drawing works fine.  

      

I'm sorry for the inconvenience it caused, will update with you when it's ready. Thanks for sharing with us! 

[PeteMwms]

It seems that the single View ISO or ASME drawings are no longer being created  everything is in 3D   so dimensioning does not work.   How do we adjust Base view to view straight on a view instead of from an angle?

[mishrani]

Hi @PeteMwms,

If your 3D model is oriented at an angle to the global coordinates, creating the base view will result in non-orthographic view.

In case, you are facing the same issue, you can try the following workaround -

1. In the design, use "Look At" (available in the bottom toolbar) then select the face of the component you want a drawing of.  You'll now be looking at that face head on.

2. Create a new named view of that orientation (Right-click Named Views in the browser) 

3. Now when you create a drawing and place the base view for component, select the corresponding named view as the Orientation in the Drawing View dialog.

This issue has been logged in IdeaStation, if you agree with the description please vote for it - 

https://forums.autodesk.com/t5/ideastation-request-a-feature-or/create-drawing-views-from-local-not-...

[nakFNE2G]

Hi,
Im having the same problem. I went through the thread and some dimensions I was able to do, but elements such as the centre marks are impossible to do. I also tried creating named views and re-stating front or top views while using the "Look At" tool for propper alignment.... but the problem persists.

[g-andresen]

Hi,
1. create a new thread
2. share the file and say which parts (and views) it is about.
File > export > save as f3 d on local drive > attach to next post.

günther