I have a drawing and want the sketches in the base view so I right click the model node under the view, select get model sketches and nothing happens. Is there a step I'm missing here? The command is now greyed out with a tick next to it but no sketches anywhere and I cant uncheck it.
Using 2011 SP0 64 bit.
Solved! Go to Solution.
Solved by stevec781. Go to Solution.
If you mean the tree in the drawing the sketches arent visible in it so its not possible to right click on them,
If you mean the tree in the part there is no option saying include when I right click.
You right click the node for the part and check get model sketches, then expand the part node, you should be able to access the model sketch.
This only works for sketches that are normal to the view.
Looks like there's something wrong as there are no sketches showing even though get model sketches is checked. All are normal to the view.
Try inserting a new base view in a new drawing and select get model sketches.
Sometimes the get model sketches fails to get the sketches if its not selected directly after the base view is inserted.
Let me know if this works.
That didnt work so I deleted the view again, saved, exited IV, re-booted machine, opened drg, inserted view and then tried and it worked. The drg was originally created in 2010 so maybe that had something to do with it.
Thanks.
I believe the command is also initially limited to Orthographic views. The context menu option, Get Model Sketches, is available if you select on a non-orthographic view, but no sketches will be displayed.
Regards,
Jerry
I have made sketches visibile (copied from Autocad) in ortho, perspective and custom view orientation with 2018 version. But it is just random success. It works one day and another it might disapear. It is nothing new, just noobie Autodesk fails, sometimes it works sometimes it doesn't..
The solution is to bring the basic view in the orthographic view( front, top etc.). Then get the sketches( they show up) and then rotate view as required and the sketches stay on.
Enjoy!
Can you provide more details, a screen capture, or a sample drawing and model please?
Regards,
Jerry
I created a handle by using the Loft command... I wasn't sure how to dimension for random points along the length. For instance, to show what the diameter should be at various points... what the biggest diameter section is and what is the smallest diameter section... The dimension command won't grab any points along the profile curve. So, I was trying to find other ways to accomplish this, but keep coming up short... I added a couple points to try to dimension to, but I can't get that to work either. Inventor Drawing won't display the points created in the model and it won't display the sketched lines created in the model either.
Not sure if it matters, but I'm on an old version of Inventor; 2011
Thanks for providing the details.
Have you tested the workflow with a new part or a different template?
Try a test with a simple part, perhaps a cube with a sketch on the top and front faces. Place the top and front views in a drawing. Get model sketches for each view and then try to Include the model sketches.
In your original part, try adding a sketch to an Origin Work Plane. Can this sketch be retrieved and included successfully?
I do not have Inventor 2011 to test the workflow.
In this thread (https://forums.autodesk.com/t5/inventor-forum/sketch-question/m-p/2921734) discussing included model sketches, a bug was discovered in Inventor 2011 and reported to Autodesk Development.
Likely you have applied all updates and service packs for 2011, but just in case, here is the link. (https://knowledge.autodesk.com/search-result/caas/downloads/content/autodesk-inventor-C2-AE-11-servi...)
I hope these are helpful suggestions. I look forward to your reply.
Regards,
Jerry
Having similar issue I've manage to get sketches working via inserting base view top down getting sketches enabling visablity. I then rotate base view to an axonometric view and enter. That seams to work and stay only if i do not update model. If i save it'll stay, but updating model gets rid of the sketch completely and then i have to annotate all over again.
Thanks! Starting with the top view & then rotating worked better for me as well on at least one drawing. Pretty buggy feature.
I have the same problem. I really don't want to remake the entire drawing. Sketching in the idw is next to useless so using a sketch in the model seems like a better option. This to is unreliable. I just want to put a bit of AutoCad geometry into an inventor idw. Why must it be so hard? Any other solutions for getting AutoCad into an idw?
Hi! If I understood your request correctly, you might want to leverage DWG Underlay workflow. Simply start a new part or open an existing part -> Import -> select the dwg file -> pick an origin plane -> pick the origin to place the dwg geometry. Save the ipt file. Create a drawing view of the part -> make the dwg underlay visible.
Many thanks!
So this issue has definitely been around for quite a while (currently on 2024), and its causes are 'bizzare' at best. Many times we create a section view that is based on a line snapping parallel, and the view draws great, then the normal to view sketches come in great. Then we save and reopen the file and the sketches are gone! So upon investigation we find that the sketch profile line rotated/tilted, even if just a tid bit, so we constrain it vertical (which is our intended view normal). BUT The sketches DON'T COME BACK!!!! Save and reopen the file, sketches DON'T COME BACK!!!
However!,
We decided to explore the events that cause the browser tree to recalculate nodes, and found that if you create a new sheet, then move the offending section view into the new sheet, the nodes get redrawn! Then we can at least include them. (they were already gotten and can not be gotten another time).
So the quickest fix to this problem thus far is to create a new sheet, move the view into the new sheet, and move it back to get all the sketch notes to reappear so you can re-include them. This is a model browser node caching error plain and simple.