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2014 OFFSET issues

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Message 1 of 28
Light_Guy
3682 Views, 27 Replies

2014 OFFSET issues

Using Inventor in 2014 Factory Design Suite Ultimate, I have run into an issue using offset in the 2D Sketch realm.

I have created geometry, a rectangle, and am beginning to add other items. I no longer require the dimensions for the rectangle so I delete them. However, once i have done that, the next item that I dimension after offsetting, causes the entire sketch to scale in accordance with the dimension I just set. I have to undo my way back to get my geometry right again and add the dims back and then I can proceed again. I have never had this problem before. Another odd thing, is that I can offset just one side of the rectangle, where normally the whole rectangle would offset. Is this new?

Paul Hamor
"Always good ships!"
27 REPLIES 27
Message 2 of 28
blair
in reply to: Light_Guy

If possible to post the file and screen captures of the issue. Possible change in workflow to add additional sketch constraints prior to deleting the existing geometry may help. As with different releases, changes to the model kernel can affect how the algorithms interpret the geometry.

 

 


Inventor 2020, In-Cad, Simulation Mechanical

Just insert the picture rather than attaching it as a file
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Message 3 of 28
rhasell
in reply to: Light_Guy

Hi

 

I have not installed 2014 yet so I can't reproduce your issue, but are you perhaps and AutoCAD user? I often see AutoCAD users deleteing their construction geometry/dimensions etc.

 

Inventor does not like uncontrained geometry, it can become unpredictable, as in your case.  Unless you specifically want the goemetry unconstrained, rather leave the dimensions inplace.

 

After selecting the Offset command, RMB and select "Loop select" option.

 

Reg
2024.2
Please Accept as a solution / Kudos
Message 4 of 28
Light_Guy
in reply to: Light_Guy

I am an AutoCAD user but have been using Inventor since the 2010 release and this is the first time I have seen this happen. I have 2011 installed on another machine and cannot duplicate this problem nor can my users who still have 2013.

Will try to post files but have not had much luck doing so lately.

Paul Hamor
"Always good ships!"
Message 5 of 28
nmunro
in reply to: Light_Guy

Your 2013 users should be able to reproduce the behavior, it is common to both. In 2013/14, if a sketch has only one dimension, changing the value of the dimension scales the complete sketch.

        


https://c3mcad.com

Message 6 of 28
Light_Guy
in reply to: Light_Guy

I'll check with them again to make sure. That is INSANE. Why would Autodesk let that go like that?? I cannot think of reason one why anyone would want that action.

Paul Hamor
"Always good ships!"
Message 7 of 28
JDMather
in reply to: Light_Guy

This was an enhancement added to 2013 release and is great.

It ensures that your sketch remains proportional after adding first dimension (entities don't end up "crossed-over").

Before this enhancement you had to get your original geometry pretty close to actual size or it could lose shape when dimensioned.  In fact, I used to recommend creating one line, arc or circle and dimension it immediately before doing anything else in a sketch to give a sense of scale.  That  is no longer needed because your sketch automatically scales for you.

 

Post back if you need to see an example why this new behavior is better.

 

As far as offsetting is concerned make sure right click Loop is active.  This is one of the few commands that does not return to default.


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Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional


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Message 8 of 28
Light_Guy
in reply to: JDMather

Please explain. It is a 2D sketch. How could it not be proportional from the get go??? I drew in a 6x6 rectangle. I am going to modify some of the lines of that rectangle later so I erase the dims. I then try to offset a line .0625 from one side, the whole thing shrinks. That makes NO sense to me.

Paul Hamor
"Always good ships!"
Message 9 of 28
SeanFarr
in reply to: Light_Guy


@Light_Guy wrote:

Please explain. It is a 2D sketch. How could it not be proportional from the get go???


JDmather is referring to the first dimension of the first sketch, I think you are having issues somewhere else down the line in the sketch environment.

 

Previously to 2013 , if you drew a "weird" shape in the sketch environment, and then proceeded to dimension, typically the initial shape you drew would end up crossed over itself. But now in Inventor, they scale this first sketch for you to avoid this.

 

I am not sure where you are having this scaling issues..

Could you attach the file to help clear up??

 

Sean Farr
Product Designer at TESInc.ca

Inventor Professional 2014-Update 2 - AutoCAD Electrical 2014
Win7-x64 | ASUS P8Z77-V | i7 3770 -3.4 GHz | 32GB RAM |
240GB SSD | nVidia GTX 670 4GB - 320.49
Message 10 of 28
JDMather
in reply to: Light_Guy


@Light_Guy wrote:

..... I then try to offset a line .0625 from one side, the whole thing shrinks. That makes NO sense to me.


Attach a file here that exhibits this behavior.  I'm not sure what you are really saying as this doesn't sound like anything I recall ever seeing.


-----------------------------------------------------------------------------------------
Autodesk Inventor 2019 Certified Professional
Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional


The CADWhisperer YouTube Channel


EESignature

Message 11 of 28
Light_Guy
in reply to: Light_Guy

OK, I see what it is doing now, still not sure why but I am guessing you guys are building far wilder things than a switch housing. Basically, because I chose to delete the dims that came in with my rectangle (because I inserted it with a specific size instead of just two points anywhere) Inventor is looking for some guidance in setting the parameters. What I need to do is change my workflow to leave at least one dim when I start a sketch.

I would upload a file but we are having issues with Windows 7 here which seem to prevent me from doing so. To see what I am dealing with, start and standard IPT file, create a 2D sketch. On any given plane, insert a rectangle with specific dims (I needed 6 x 6). When you insert a rectangle with specific size, it inserts the dims automatically. Erase those dims. Now offset a line to either side of the rectangle. That line needs to be 1/16th of an inch away so you dim that distance. Because there are no longer any dims on the original rectangle, it shrinks both rectangles to suit that 1/16th dim.

I still need an example of why that is a good thing just to wrap my head completely around it, but at least now I know what I need to do to carry on.

Paul Hamor
"Always good ships!"
Message 12 of 28
SeanFarr
in reply to: Light_Guy


@Light_Guy wrote:
Erase those dims.

Why do you need to erase these?

Sean Farr
Product Designer at TESInc.ca

Inventor Professional 2014-Update 2 - AutoCAD Electrical 2014
Win7-x64 | ASUS P8Z77-V | i7 3770 -3.4 GHz | 32GB RAM |
240GB SSD | nVidia GTX 670 4GB - 320.49
Message 13 of 28
Light_Guy
in reply to: Light_Guy

Because I am going to modify those lines in a couple more steps and Inventor will force me to delete the parameter before I can do that. Its a forward thinking step which, I guess I need to quit doing.

Paul Hamor
"Always good ships!"
Message 14 of 28
sam_m
in reply to: Light_Guy

are you sketching like AutoCAD - trying to draw with the correct dimension, using direct input, before actually dimensioning?  therefore believing you've drawing a 6x6 rectangle and the 1st dimension you place is the 0.0625 offset and the entire sketch shrinks - is that what you've explaining?

 

if so, then remember Inventor is not AutoCAD and you don't need to draw specifying (@6,0) dimensions, like AutoCAD.  Just draw the shape of what you want (without needing to worry about its dimensions) and then you dimension it to fully define the shape, offset and dim that and ensure it's all fully constrained.



Sam M.
Inventor and Showcase monkey

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Message 15 of 28
Light_Guy
in reply to: Light_Guy

That is exactly what is happening. Normally it doesn't come back to haunt me but since I needed to put breaks in the lines that make up the rectangle, I had to delete the dims before it would let me do that. It's all about retraining the brain to think abstractly instead of orthagonally.

This is set up for creating "new" things, I am bringing my old 2D world into the 3D world so I am creating 3D parts from existing 2D drawings and already have all the dims I need.

Paul Hamor
"Always good ships!"
Message 16 of 28
JDMather
in reply to: Light_Guy


@Light_Guy wrote:

Because I am going to modify those lines in a couple more steps and Inventor will force me to delete the parameter before I can do that. Its a forward thinking step which, I guess I need to quit doing.


I still don't understand why you need to delete dimensions or why Inventor would force you to delete parameters, but anyhow - carry on.

Well, I'm still trying to get my head around this.  If  you don't want the dimensions why take the extra trouble of entering them in the first place?  To get appoximate scale (actually, exact scale as you are entering the dimensions)?  You don't need to do this.  I'm still kind of confused, but it looks like you have it figured out for your needs.


-----------------------------------------------------------------------------------------
Autodesk Inventor 2019 Certified Professional
Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional


The CADWhisperer YouTube Channel


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Message 17 of 28
SeanFarr
in reply to: JDMather

I am confused as well, however it seems that it is related to AutoCAD and I don't know too much about that software...must be some workflow he is used to and trying to adapt it to Inventor...

Sean Farr
Product Designer at TESInc.ca

Inventor Professional 2014-Update 2 - AutoCAD Electrical 2014
Win7-x64 | ASUS P8Z77-V | i7 3770 -3.4 GHz | 32GB RAM |
240GB SSD | nVidia GTX 670 4GB - 320.49
Message 18 of 28
Light_Guy
in reply to: Light_Guy

The rectangle was my outer most boundary, which I knew to be a specific size. Because I had to make some breaks in those lines, I was blowing away the dims in advance of Inventor telling me I had to. I was thinking several steps ahead and tripped over my own feet I guess you could say.

Paul Hamor
"Always good ships!"
Message 19 of 28
SeanFarr
in reply to: Light_Guy

When I need to create a part within a specific boundary, I typically use construction lines, you can leave dimensions on them and then add you other geometry to the sketch and keep it within the boundaries or use as a reference for dimensioning.

 

constructionlines.png

Sean Farr
Product Designer at TESInc.ca

Inventor Professional 2014-Update 2 - AutoCAD Electrical 2014
Win7-x64 | ASUS P8Z77-V | i7 3770 -3.4 GHz | 32GB RAM |
240GB SSD | nVidia GTX 670 4GB - 320.49
Message 20 of 28
rhasell
in reply to: SeanFarr

Okay so we have determined that there is a workflow issue, and some AutoCAD habits cropping up, very difficult to "Un-learn" But the scaling of the part with the first dimension placed is a God send and saves many frustrating hours of re-doing sketches because they fell apart due to incorrect scale.

 

Did you fix the Offset Loop issue?

 

Reg
2024.2
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