Offset assigning random values in sketch mode

[davidfarmer]

I use the offset function in sketch mode quite often, and  about a month ago this issue started happening. I would select the offset tool, then select a line and type in the value I needed to offset. in this case its always 0.375". then I press enter and it makes the offset line. The line then displays the dimension next to it and it is not the value I typed in. The line is also not offset the correct amount. I then double click on the dimension and the number is what I had typed in, then I press enter and it snaps to the correct dimension. a couple weeks ago I reset my computer and reinstalled all the programs including inventor 2016 and Vault and the problem went away. yesterday it started happening again and its also happening to my coworkers now. I started just assigning the value I want to offset to a variable, b for example, and then just type in b every time and it does the same thing, however I can use the ilogic form or the parameters table to change the value of all of the offset lines at the same time, but its still very frustrating. I have attached step by step pictures of when the issue occurs.

[Giordanik]

Dear davidfarmer,

That is certainly irregular. Could you post the part file (.ipt) for examination?

[davidfarmer]

ok heres an attached part. also notice how it only happens on the offsets not on any other dimensions.

[Daniel248]

I've tried to reproduce your issue, but without success (SP2 installed here).

When entering an offset in that box, the resulting offset and dimension are correct - have a look below at my screenshot steps:

Looking at the product version you've used for this part, it seems like you have not updated Inventor with the latest service packs, and you're still on

SP0 build=138;ProductVersion=200138000

I suggest updating Inventor with the service packs, and then try again to see if you see the same problem - maybe this has been fixed by an update;

Spoiler

Using a background image in Inventor could slow things down a bit, and doesn't help when trying to see clearly - I know, it's a personal choice and there's nothing wrong with that - I like mine clear and simple...   

[AMRIT9988 · Accepted solution]

goto app options>sketch>de-select snap to grid. 

All will be fixed. 

you clicked the little grid symbol on the bottom of the screen while closing tabs down.

still have questions call me

631 662 7686

[davidfarmer]

Thanks a lot, thats been bothering us for weeks!

[AMRIT9988]

bothered me for 45 minutes until i figured it out. ahaha

[Curtis_Waguespack]

Hi everyone,

Hmmmmm, I just tested this with the grid snap on. My snap spacing was 0.100 cm. I was seeing varying results, none of which were very consistent or expected.

With the grid snap on, when I tried to offset a line I saw:

• the offset dimension jumping to the snap distance, rather than the value typed in
• the displayed offset dimensions not matching dimension in the dimension edit box
• sometimes the value off the offset did follow the typed in value if I pressed tab first (maybe?)

I wonder if @johnsonshiue can have a look and tell us if this is working correctly?  or if there is something not quite right here?

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[Jacob_Butler]

I was just checking to see if I get this same issue too and experienced some weird results as well.

[davidfarmer]

just curious but how did you make that video?

[Jacob_Butler]

Hi David, visit this link: https://knowledge.autodesk.com/community/screencast

[johnsonshiue]

Hi! I am able to reproduce the behavior. This is a bug. When Grid Snap is turned on, if the user enters an offset value not equal to the snap value, the entered value will be recorded in the parameter expression but the nominal value is actually the snapped value. This is wrong. I am able to reproduce it on 2015 and later releases. I will work with project team to resolve the issue. Many thanks!

[davidfarmer]

Hey while your at it can you fix the midplane function in assembly mode? currently you cannot make a midplane using two faces from one part. my work around is to make an offset plane first, then use the midplane function.

[johnsonshiue]

Hi David, Let me explain how mid-plane workplane works in assembly. Assembly work geometry is actually considered components as opposed to features in a part. You might notice that all of assembly work geometry carry assembly constraints after they are created. In this case, mid-plane is leveraging symmetric constraint. Symmetric constraint requires two different components and a plane. As a result the components need to be different. They cannot be the same. Is there a reason why such mid-plane could not be created within the part of interest? This thread was intended for the sketch offset issue, not for mid-plane workplane. You might consider starting a new thread. Many thanks!

[Curtis_Waguespack]

Hi davidfarmer,

1. While there are some Autodesk employees, such as johnsonshiue that visit these forums, and investigate and report bugs, the process of getting those things fixed is a bit more involved, and generally will happen via new product releases or service packs and update releases.
2. The proper method to request improvements is currently the Idea Station. Where you can share your ideas about how to improve Inventor with the development team:
   http://forums.autodesk.com/t5/Inventor-IdeaStation/idb-p/v1232
3. The work plane issue you're talking about, is not a bug, but just a limitation in how it works. If you search the IdeaStation, you might fine an improvement request for the ability you're asking about already logged, if not you can create one.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[masterkreek]

My colleague has come across this issue as well in the 2018 release. I have always had snap to grid turned off but he didn't. Thanks for the help from this forum for diagnosing the issue.