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I've tried finding a solution to my problem here on the board without success. Hopefully someone here has an idea...
I have an assembly drawing that I'm demsioning, but some of my dimesions are displaying incorrectly. Instead of displaying as if I was I was dimensioning from face to face when I choose 2 lines, it's dimensioning from edge to edge.
I've checked my parts, constraints and views, and everything seems to be square.
This Post explains what is happening. Somehow, my General Dimension Type (found by right-clicking each view in the drawing) began defaulting to "True" on sheet 24 of a 24 sheet DWG. No idea how or why! It is set to "Projected" on the first 23 sheets, but now, every new sheet I create defaults to "True".
Any ideas how to switch the default back to "Projected"?
Can you log on with another users credentials and try to repeat the problem?
Sometimes associated files can become corrupted (a 1 where a 0 should be, hotfix cuases etc) and cause these types of anomalies. It is a relatively easy fix but you will have to try different log in details to verify if this is the problem.
Chris, good recommendation. Now that I think about it, this issue manifested after Inventor crashed while working on this file.
However, a different login does not help. Same issue.
I am reading that Inventor should default to the proper General Dimension Type depending on view type. For example, ortho views should default to Projected, and iso view should default to True.
On this particular assembly, that is not the case. Each part defaults correctly, but the assembly does not.
From your last post I would strongly suggest that yes, your assembly file is what is causing the issue.
I have a batch script that will reset your Autodesk profile information which resets all your Autodesk applications to default like the day it was installed but I do not think that it is system files if changing user did not resolve the problem.
Try editing the assembly slightly (add/remove a part, change a constraints etc) and then resave and start a new drawing file with the newly saved assembly. If there is an issue with it this should solve the issue. If this does not resolve the problem then you may have to recreate the assembly.
Unfortunately, changing the assembly does not correct the issue.
On the plus side, this is the last sheet of my drawing package, and now that I know to switch the General Dimension Type to Projected, I can at least finish my project.
I'm going to leave this issue open, and maybe someone can give an explanation as to why this assembly is defaulting incorrectly.
Kudos to you, though, for all your recommendations! Hopefully, there's a logical explanation that will help us better understand what's happening.
Are you having the same problem with newly created parts/assemblies? or is it just specific to this.
Have you checked to make sure your assembly is square to the origin planes?
Have you tried to place a new view and use the "change view orientation" button along with the look at face to ensure your views are square to the assembly?
are you able to pack and go the assembly and post it? This will give me a better chance of diagnosing the issue.
I have attached the script to reset the Autodesk profile which will reset all the styles, options etc if you wanted to try that instead. You will have to change the .txt to .bat for the script to run.
The script effectively removes all the options data and saves it outside of the folder the application reads it from. Depending on your software version you will have to remove 'rem' from the beginning of the script. It is currently set for 2015 software.
I had not considered constraining the assembly to the origin planes. This is first time I've had this problem. I did so, and the drawing defaults properly. Thank you, mcgyvr.
Here's what I did:
Constrain the assembly to all (3) origin planes.
Reset the model view by using "Page Up" on the keyboard, selecting a face and right-clicking the viewcube to "set Current View as" front.
Created a new ortho view in my drawing, and voila! The new view's "General Dimension Type" defaults to "Projected", as it should.
Is it best practice to constrain all parts and assemblies to the origin planes?
To be honest I never though about the assembly not being grounded as this is usually the first thing I do when I create assemblies. Go to show, the easiest solution is usually the right one 🙂
Just so you know for next time if you right click the mouse instead of left click when placing your first item there is an option to "Place grounded at origin" which will snap that part to the origin planes and ground it so it is fixed there.
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