Hi,
I am struggling with projected geometry that is for some reason not updating in sketch when I change sorce element.
I have sketch in ipt file A.ipt
A.ipt is placed in A1.iam.
in A1.iam I create or place B.ipt
in B.ipt I create sketch and project some elements of A.ipt sketch to it.
After any change i sketch in A.ipt file I and up with elements projected to sketch in B.ipt not muchning elements they ware projected from.
I tried I think everything, adaptivity, creating additional points i A1.iam (they update properly but still projection is not updating).
What is wrong?
Regards,
Cris
Cris,
I find a lot in my usage of the software it does not update a lot. It is frustrating at times.
It sounds like you are creating a derived part in the assembly.
Have you tried using the rebuild all command under the manage tab?
Cris, I try to avoid projected geometry whenever I can. Sometimes I will project a feature to another part, but I open the projected sketch and manually add the geometry making sure it is fully constrained and dimensioned, then I delete the projected geometry. It's more work, but it saves from having the problems you are reporting. It's not always foolproof though
I assume you are using 2013?
With your projected geometry, do you find that it doesn't update, but instead the projected geometry breaks (IE: lines and points turn pink instead of green or blue for a constrained sketch)?
The colors mentioned are dependant on the color scheme you are using, I use 'Winter Day', and the actual colors may be different in some of the other schemes.
Andy,
I am still using 2012. I personally hate the projected geometry command as well. Almost see no reason for it.
But with that said is this command different in 2013?
I have used the command in the assembly environment and not experienced what is being described here.
Scott, I have seen this in 2012 SP0, possibly SP1 also, but to a much lesser extent than in 2013.
I did raise this problem here somewhere, but I haven't had the time or seen the problem whilst remembering to capture it ... lol
It also happens in the part environment, but in that case I usually end up with broken geometry/features because the sketch is broken or now has a missing axis or plane. It gets real annoying when you have to go back and fix geometry that should not have broken in the first place, but has.
I will document this in a video just as soon as I encounter it again and have the presence of mind to do so, don't hold ya breath though ... lol
@Cadmanto wrote:Andy,
I am still using 2012. I personally hate the projected geometry command as well. Almost see no reason for it.
I am still using 2012. I personally love the projected geometry command and have probably used it on every single part I have ever modeled in Inventor, SolidWorks and Pro/E (Creo). I (almost) never project geometry in assembly environment though. I prefer to use Derived Components (prior to 2010) and now mutl-body solids over assembly in-context adaptive geometry.
The CADWhisperer YouTube Channel
Hi all,
I see this topic has quite a responce.
To ansewer some questions.
- Yes what I am doing is similar to derivered part. But I thought I could just project parts of sketch instead of derive big sketch from sorce.
- When I change I got geometry in sketch changed to "fixed (locker icon)" constrain from projected. No mather what level of update I do
- in the same time projected edges of solid elements are updating, as long as their "number" in databes is not changed. When particular edge is altered it ofcoures is after lost in sketch projection and marked in purple/pink
What I would like to chiewe:
I would like to define base sketch in surce file and aftre in assembly file create diferent elements basing on this sketch. I wont to do this in the way that when I will make some changes in base sketch rest will update acordingly.
Currently I am designing trus and in the same time have to design and calculate, and constantly make some changes in geometry.
Regards,
Cris
Its quite possible that you arent doing anything wrong. I often get sketch references fail to update after minor changes that dont change topology, just dimensions. I have lost count of the hours wasted fixing sketches that break for no reason.
I used to use cross part projection but hoping for more stable models I moved to deriving parts in as composite and deriving sketch geom from them so that the derive is fully withiin the part. Just today I wasted 2 hours because the sketches all broke even though the derived component updated correctly. There were no topology changes, just a change in height. Its always the end points of lines that fail to update.
Dont forget Inventor is not fully parametric, if you use Project Cut Edges across parts the lines with be fixed and non parametric. This is standard. Same if you project a sketch from one part into another. It will be fixed and non parametric.
I don't think so. Project Cut Edges is parametric and updates as expected. At least since IV2010. It used to be non parametric in earlier releases.
Regards,
Igor.
@stevec781 wrote:
Dont forget Inventor is not fully parametric, if you use Project Cut Edges across parts the lines with be fixed and non parametric. This is standard. Same if you project a sketch from one part into another. It will be fixed and non parametric.
Straight from the 2013 wiki help.
You can project the edges of a component cut by an assembly section to the sketch plane if the part would intersect the sketch plane. Projected cut edges are not associative in a sketch. The geometry is a "snapshot" of the geometry when projected, and if the parent geometry changes, does not update
For sketches its the same you can easy test. From within and assembly create a sketch in part A, make it visible. In part B create a new sketch, use project geom and select a line from the sketch in part A. The line that appears in the sketch in part B will be locked and not associative just as the OP describes.
I see. The phrase 'in assembly" has escaped me. I never build anything from within the assembly file. I use "bottom up" approach instead. On part level "Project Cut Edges" is as parametric as it should be.
Regards,
Igor.
Actually, sketches from another part can be associatively projected into another part sketch. See picture included highlighted two places in the browser and the corresponding constraint in window.
Edit; To be clear I am refererring to Inv2013sp2upd5
I know and many others knew what you meant but it was not what you stated here:
"For sketches its the same you can easy test. From within and assembly create a sketch in part A, make it visible. In part B create a new sketch, use ***>project geom<*** and select a line from the sketch in part A. The line that appears in the sketch in part B will be locked and not associative just as the OP describes."
It might be beneficial to edit your statement from ***>project geom<*** to ***>project cut<*** as you stated previously.
Attention to details and accurate information is what people are looking for. It is especially required when it comes to commands, differences of versions, skill of the user, or doing what it is we do with these applications.
Edit: formating chg.
My post was written in 2012 and both were an issue then. Below is a screen shot from back then. Glad they have fixed one of the issues that was a big problem for me since ver 2010.
Just checked the 2015 help and project cut edges are still not associative when done at assembly level.
They finally fixed something that has been missing from the beginning. When they made it so that sketch entities could be projected to other parts and retain the association.
Hi! Something either is not working right or there could be cycle among them. Could you provide an example here or send it to me directly (johnson.shiue@autodesk.com)?
Many thanks!
@VeeGee wrote:They finally fixed something that has been missing from the beginning. When they made it so that sketch entities could be projected to other parts and retain the association.
If you knew it was a problem from the beginning, why did you dig up a 2 year old thread ?
I dug up a two year old thread to correct something that another wrote so as to not continue to misguide others. You know, your incorrect statement.