Hey everyone, for some reason I am having all kids of trouble generating the G code for this park using sketch U cam. I have been following marks tutorial and its just not working at all. I am unable to select inside and out side cuts for this part. I have expanded and flattened just like I am supposed to. Any help would be greatly appreciated! Thanks. P.S I have attached the file I am working on.
No, it is not flat, it is a 3d part. It also has a lot of hidden geometry which is interfering with the Phlatten tool. What I did: copy and paste the bottom face of the object. (to avoid the hidden geom interfering) position the safe cut area put center points in the hole positions (I have a plugin for this, google it) select all the 5mm holes and create a group select all the 7.14mm holes and create a group (the above groups prevent the drawn holes interfering with the plunge hole tool) select the SketchUcam plunge hole tool press HOME enter 5 and press enter click the center points of all the 5mm holes in the order you want them cut press HOME twice enter 7.14 and press enter click each of the center of the 7.14mm holes, in order you them cut select outside cut tool apply outside cut to the face. generate Gcode you will need to cross check your material thickness, feed speeds, and bit diameter. if you change bit diameter from 3mm, you will need to delete and redraw the outside cut. if you are cutting aluminum, set stepover% to 30% - and set hole cutting mode to 'diam first'. (how to do that IS in the help, recommended reading). Maybe Marks tutorial needs updating? Please link it so I can check. This is much more current, along with other videos I made about the new features I have been adding.
trying again , nope, @Mark Carew I keep getting an error when uploading a sketchup file. use this link instead @CCV http://iwr.ru.ac.za/~david/phlat/XZ_Plate_14_Wheels.skp
Thanks for the help. I now see where I went wrong. The bit i am using is slightly larger than 3 mm so I changed the specs and re made the outside cut. One thing I cant find is setting the hole cutting mode to diameter first. I referred to the help section like you mentioned but could nit find anything in there for setting the hole cutting modes as this will be cut in aluminum. Here is a link to the tutorial that I was following before:
sorry, my bad, you have 1.4 and I have changed stuff since then for the 1.4a release.... (coming soon, beta testing in progress) so yours looks similar but does not have the subcategories under 'Change default options' so click that, then scroll down to 'hole feature options' which is on that page.
It all makes sense now, the version of sketchucam that I had was older and did not have hole feature options. I deleted a installed version 1.4 and am now golden. Thanks for the help David!
