How can this part be thickened by 1mm internally?
The thicken quilt works upto 0.9mm but an error is seen at 1mm.
The preview appears in green - how can I find the feature which is stopping the operation?
Why not change the dimensions of the features in question. Like subtract 1 mm from each of the circles in the sketches 4 through 10 in the loft.
Thanks for posting this - I shelled the original part that you attached as testpart100.ipt to 0.9mm (shell/thicken both use offset algorithms) and opened faces of the large base 'box' to leave the feature-rich top face. I then flipped the part over using the view cube to give the view below:
Labels A,B,C,D refer to vertices (where A and D lie outside the area of the red box). The feature preventing the offset at 1mm is the small circular face in Sketch4 that was used to create Loft1. As the offset distance is increased, the partially ghosted arc BC gets larger and chord BC vanishes to zero. When chord BC finally reaches zero, vertices B and C coincide. This offset 'event horizon' lies somewhere between 0.9mm and 1mm and causes a large topology change, resulting in the error that you observed.
In order for the offset to succeed at 1mm you could make the small half circle in Sketch4 bigger.
I'm working on another idea I have which involves changing the shape of Sketch4 and I'll let you know if it's successful - in the meantime I hope this has helped!
I think I have a workaround but I admit it's far from elegant..! It involves changing the shape of Sketch4 as I mentioned in my previous post but also the shape of the other circular sketches in the loft.
I've 'squared off' the circles where they meet Extrusion1 and this allows the shell/offset to succeed at higher values than it did before. Hopefully the image below makes my words clearer:
In effect, it's an arch with short upright straight edges (Architects, please forgive my poor terminology), in this case of 0.5mm.
Please note that in order to steer clear of creating sliver faces and therefore tolerance issues, I created this upright on all sketches consumed by Loft2 in the attached part file.
As I alluded to earlier, there could be a more elegant workaround: this is just an idea I had.
Feel free to give a shout