FreeCad Loses my Sketch when it is closed

I built what I thought was a successful sketch, but when I hit the Close button to use the Pad feature my sketch disappeared. I have to scroll the build area of the screen until a small green dot appears, and eventually the sketch will expand and it eventually comes back. However; you can not use pad or anything else because as soon as you hit close again, the sketch disappears. I see others have had this problem, but found no results. I tried the full screen button, turned a lot of the true/false options to true in the view and data property panes. Any help would be appreciated.

First, it is hard to follow without seeing anything. Maybe upload some pictures to show what is going on.

First of all. If you hit close the sketch is only “gone”, when it is invisible, far back (out of scale) or simply turned invisible. On the left side is the combo view. It should show the sketch you just created. Usually FreeCAD switches to “task” or something on the left, but you can simply select the tab to get the tree view behind again.

To check if the global view is out of scope just right click, in the model view (after clicking close). In the popup menu is an item called “make fit” (or something like that (I am using the german version most of the time, but tried english, too but my be remembering wrong). This option should scale the main view, so the model you are making is actually in the scale of the screen.

If your sketch still isn´t shown, check the icon next to your sketch in the list on the left. The picture should be solid. If it is fainted or transparent looking, it got disabled for some reason. To make it visible you just make the entry of your sketch active and hit space.

To create the pad the sketch itself does not need to be visible at all. You just need to select it and hit the pad option. Usually, when using the pad/pocket or what not button in the “Task” section after closing the sketch editor, if should already be selected.

If the scale is wrong, you off course won’t see the padding, as it is in the same scale and may be to far away or to zoomed in. Use the “make fit” option in the context menu to get it centered on screen. You need the context menu of the model view. This is important. Each section has own menus here.

As said this is only a wild guess as I cannot see what you see and words can be confusion here. :smiley:

I have included a PDF file as to what I encountered while trying to build from a sketch. The original being, after my Sketch is drawn and after I select the close button, the sketch disappears from the build screen. I hope it provides enough information. I can always get more if you need it.

FreeCAD_Issues.pdf (733 KB)

The first photo would have been enough.

Your sketch is not valid to be padded.

There is a simple rule to ensure a sketch is valid for creating a pad or pocket:

If you use scissors and cut around all lines, then you must get the shape you want in one piece.

In your case you get multiple shapes. Sketches define the outer shape you want to create. In your case this is not possible. That is why the Pad icon has a red “!” next to it.

If you turn the inner lines of your sketch into construction lines (or helper lines which I think is a better wording), the sketch get valid for being padded. Just multi-select the inner lines and click on the icon with the two squares hovering above each other. Usually more or less the last in the draw section, where you find the line tools. This turns the selected lines into a blue version.

Referring to the rule you just made the inner lines irrelevant for the scissors. Kind of like dotted bending lines in paper models.

The blue line is only a design helper line or construction line. It never gets used to create a shape or other stuff, but helps positioning the normal lines and can be constrained in the same way. It is a powerful tool to simplify your model.

You may ask why FreeCAD is not reporting your sketch as invalid. Well, the sketcher can be used for many other operations and some of them may allow them may support stuff. For example a single line is not valid to create a shape (see rule above), but for operations that extrude another sketch along the line in the this sketch, the sketch is valid.

Another thing you should know about FreeCAD: If something turns invisible after an operation, it is usually caused due to some impossible geometry or action. This is a design flow of FreeCAD. It should be more pointing onto the real issue here and not confusing the user by making him feel he just lost his work.

Usually there is an error or a tiny hint. In your case the little red “!” over the icon of the pad. You can work on your model, but as long as there is a “!” anywhere in the list, nothing will be shown anymore, so make sure to solve the issue before you continue.