Quickly delete reference geometry

[Anonymous]

I'm finding this to be slow part of my workflow. Any tricks on making to workflow faster?

1. Cross-feature and cross-part references are very fragile (shouldn't this be better in 2017?)

2. I end up spending a lot of time deleting broken geometry and pink lines.

3. Deleting reference geometry usually involves 3-4 right clicks to select the lines, select the references icon, delete the ref then the lines

Questions:

1. Surely references could follow geometry changes better. Beyond waiting for software improvements, any better way to manage it?

2. Any way to bulk delete all projected geometry from a sketch, leaving the drawn lines in-place, so I can re-constrain it?

3. Any special option key that allows me to immediately delete a line, without fussing around with deleting its references first?

[Thomas_Savage]

Hello,

Could you attach one of your files please?

If you are having problems with projected geometry, and losing the projected geometry, you could be sketching incorrectly.

Someone on this forum the other day was having a problem with losing projected geometry of a line, and it going pink. And it was because he had not constrained the line to the edge correctly. So when he changed the thickness of the shell, it lost reference, and went pink. Once I constrained the line to the edges correctly, there was no problem.

Or you could be deleting a feature, and losing the projected geometry. Which causes it to go pink.

If you sketch correctly you should have no problems with losing projected geometry, and your lines going pink.

Thomas.

[johnsonshiue]

Hi Troy,

I am not aware of a systematic issue slowing Inventor down due to using projected geometry or reference geometry. The behavior you describe here does not sound right to me. Could you provide an example exhibiting the behavior (or send it directly to me johnson.shiue@autodesk,.com)? I would like to understand it better.

Many thanks!

[Anonymous]

Here is the cross-part break from a minute ago:

It is sliding tensioner that travels down a slot and hole. This part was fully constrained to the projected reference geometry of the hole and slot using an offset.

All I did to break it was re-deminsion the original hole points to move them 0.020" lower (using the same feature, sketch & points). The reference part updated, but the projected lines broke. Happens all the time. As you can see here (notice the reference geometry all moved with the hole change, even edges not affected by the move):

[Anonymous]

Its not inventor slowing down, but the painfully slow UX/UI design.

Trying to delete references is super fidgety at best. Considering it breaks all the time, I bet I spend 30% of my inventor time deleting and redrawing broken reference geometry.

Inventor makes you select reference geometry 2-4 times per segment to delete a line. Half the time it doesn't even show a delete option, and you have to click away, then select again to get it to come back (see video).

Line...by...line...by...line. Could they make this any more slow and painful? There has to be a faster way to select reference only geometry as a group and hit delete -no questions asked - without having to click...every...reference icon...twice...then...delete...the....line.

see video for example

[johnsonshiue]

Hi Troy,

You could right-click within Sketch environment -> Show All Constraints. Then you could window-select the constraints to delete. However, the existence of pink sketch geometry indicates something is not working right. It means the associativity between the sketch geometry and source geometry is gone. Did you delete the source geometry intentionally? If not, I need to see an example. This does not look right to me.

Many thanks!

[kelly.young]

Hello @Anonymous I am responding to your selection of the Project Geometry issues:

When editing the Sketch select all the lines at once, it should bring up the constraints and Projected Geometry symbols.

Drag the Projected Geometry symbol a tiny bit, then hit Delete or RMB Delete. Makes it much easier.

Also, you can go to the Browser Tree, find the Sketch and click the > to expand showing the Projected Loop and delete from there.

The drawing practices which are breaking your reference is another issue that @Thomas_Savage and @johnsonshiue were addressing well and should be investigated further.

Please select the Accept as Solution button if a post solves your issue or answers your question.

[jtylerbc]

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kelly.young wrote:

Also, you can go to the Browser Tree, find the Sketch and click the > to expand showing the Projected Loop and delete from there.

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Slight correction to Kelly's description:  In a cross-part scenario, it won't say "Projected Loop", it will say "Reference#". 

"Projected Loop" is what it would call the equivalent browser entry for when a face is projected from within the same part (no cross-part geometry involved).  It behaves pretty much the same, but in a different context.

Aside from the little terminology nitpick, this is what I would suggest as well.  There's no need to delete the Projected Geometry constraint, then delete the actual geometry in a second pass.  You can just delete it all from a single action in the Browser - I just didn't want you to get hung up looking for the wrong name.

[Anonymous]

The browser delete is good approach, but it only shows up in cross part projections. WIth-in the same part, there isn't a a list of projected references. So it only works some of the time

[Anonymous]

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@johnsonshiue wrote:

Hi Troy,

You could right-click within Sketch environment -> Show All Constraints. Then you could window-select the constraints to delete. However, the existence of pink sketch geometry indicates something is not working right.

---

Is there a way to only group select/delete the reference geometry without grabing the drawn geometry. Usually they are very close to one another.

[jtylerbc]

Technically true.  But within a single part you can just delete the geometry directly (by selecting it in the sketch and hitting the Delete key), so it doesn't really matter that you can't delete it from the browser.  You simply don't need to.

The only time I'm aware of in a single-part scenario where that doesn't work is the "Projected Loop" scenario mentioned earlier.  In that case, it does show up in the browser, and works the same as deleting the "Reference#" entry from a cross-part projection.  

[kelly.young]

@Anonymous You seem to know how to select the lines, I would again recommend selecting all and finding the Projected Geometry glyph like I stated before, if the lines are close that helps.

RMB > select other... will pull up a list of lines that may be on top of each other.

Let's now focus on how you are linking the parts and why they are breaking to give you the pink lines.

Can you show a screencast of what you are doing to break them? I think your setup and workflow is causing the error as they should not be breaking if setup correctly.

[Thomas_Savage]

Hello,

Would you be able to attach your part?

So I can have a loo at it.

Thomas.

[Anonymous]

Thanks for the offer. I'm not allowed to upload the original. Unfortunately when building simple example files, i can't reproduce it. References work well in trivial examples. But when built up into complex parts having dozen of features, things get fragile.

Is this not a other peoples experience?

[kelly.young]

@Anonymous the main reason things get fragile is that constraints are broken. When an associative part changes in size the projected geometry is pulled through. If it changes to where there are new lines created or necessary lines removed that is when they break most often.

There are many different ways to model and depending on what you're trying to achieve there might be a less fragile way to go, are you familiar with using derived parts instead of associative parts?

Much less fragile as the actual derived model is being referenced not pulled through associatively.

Please select the Accept as Solution button if a post solves your issue or answers your question.

[Anonymous]

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@kelly.young wrote:

@Anonymous the main reason things get fragile is that constraints are broken. When an associative part changes in size the projected geometry is pulled through.

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Are there projected geometries more susceptible to breaking than others? Are there types of cross-part projection that are more fragile?

Does it matter if you project perpendicular to the original features sketch (thus referencing the user draw sketch), versus projecting an edge generated by a 3D feature process?

[Anonymous]

I am having the exact same problem very often. Tons of time in my bachelor thesis has gone to try to get rid of pink lines but they are not easily deleted and I have to click many times. I attached one of the parts. Sketch 23 is now causing trouble. I started to break link at every use of project geometry but lately the break link is not an option anymore. In my opinion the autodesk inventor professional is still in the stone age as far as user friendly goes.

[kelly.young · Accepted solution]

Hello @Anonymous thanks for attaching the part, much easier to give feedback.

Here is a short screencast showing how to Redefine Sketch and Break/Delete Projected Geometry Link.

Hope that helps!

Please select the Accept Solution button if a post solves your issue or answers your question.

[Anonymous]

Thank you for your help!