Trying to pad a sketch drawn in a hole

[jswild]

I've been fooling around with it and found out that the problem does not seem to have anything to do with positioning the sketch for the dowel over the hole. Even if I place a fully constrained circle over a solid piece of the upright, it still will not pad (or pocket). When I try to pad I get the same message I reported in my previous post. If I try to pocket the message is "Please create a sketch or 2D object first. It must have a support face on a solid."

But, since I selected the face of the upright to sketch on, how can the sketch not be on a support face?

Jim

[jswild]

Even more...I have tried to pad from sketches on many surfaces in my project, but none of them can be padded from, for the same reasons noted above. It's like my whole drawing has been coated with teflon and nothing will stick to it. That just sounds weird to me, but maybe it is a clue someone who knows more.

Jim

[GeneFC]

Jim,

The problem in the latest file you posted is very simple. You left the circle in Sketch004 as construction geometry (blue) instead of ordinary geometry.

Select the circle in the sketch, toggle the construction geometry icon, the circle turns green, and you can now pad the sketch without difficulty.

By the way, all of the circular dimensions are in terms of radius, not diameter. It does not change any of this discussion, but you may not have the sizes that you desire.

Gene

[jswild]

Thanks Gene.

I don't know why the circle was construction geometry. Is there some way to change the state of the program so that everything you draw is CG? If there is, I must have triggered it.

Would you comment further on what I have done? Specifically, in my model view there are five objects. The first three are grayed out in the list. I can still access them and even edit their underlying sketches. Does being grayed out in the list signify something?

Also, now that I have padded the dowel into existence, the slots it fits into have been filled in around it.

pic01.jpg (11.99 KiB) Viewed 1511 times

And, when I click on a face it does not turn a uniform green but has a strange pattern in green on it.

pic01.jpg (11.99 KiB) Viewed 1511 times

Are these things just artifacts of the display or do they indicate I'm headed for trouble again?

Thanks,

Jim

[chrisb]

I don't know why the circle was construction geometry. Is there some way to change the state of the program so that everything you draw is CG? If there is, I must have triggered it.

If you ever change to construction geometry (icon with red and blue square) all following geometries are in construction mode until you toggle it again. You see it immediately: colour is blue.

The first three are grayed out in the list. I can still access them and even edit their underlying sketches. Does being grayed out in the list signify something?

greyed out is good for you! It means that this previous state is not displayed. If you have more than the last state visible you are likely to fork your model, which is not good. If I work on a previous state I usually make only that state visible. After editing I change immediately back to have only the last state visible.

Also, now that I have padded the dowel into existence, the slots it fits into have been filled in around it.
...
Are these things just artifacts of the display or do they indicate I'm headed for trouble again?

It is already explained: You see the object with pockets and without at the same time, which means you don't see the pockets

[GeneFC]

Jim,

Adding to what chrisb said, the construction state is indicated by all of the drawing icons in the toolbar turning blue. Once you understand that behavior, it becomes obvious when you are in full-time construction mode.

Gene

[jswild]

Thanks, Chris and Gene.

I've "finished" my design and attach it here. I'm rather pleased with myself since a week ago I had never heard of FreeCAD. However, I put finished in quotes because there are a couple of things about the design that are not quite right.

1. Chris explained about the model elements being grayed out and so now I want them all grayed out. However, Left Support Dowel and Pulley are not grayed out. I don't know why. The last element, Braces, is not grayed out, as expected, but it is also bold. Significance?

2. The Support Dowels were put in place by making a sketch on the front face of the left upright and creating circles which were then positioned hovering over the Main Dowel and padded in two dimensions to go down into the Main Dowel and outward into space. I tried making both circles in one sketch and padding them, but that didn't work. Usually I got only one of them created. So I did each of them in a separate sketch and that works pretty well, except that sometimes in later stages of working, one of them will disappear until I edit the pad operation that created it. I don't change any pad parameters, just click OK and it pops back into view. This may be related to the not grayed out state of Left Support Dowel.

3. The Pulley element is not exactly centered on the axis of the Main Dowel. I created its sketch in the XY plane and set it on the Main Dowel as closely as I could by eye (external geometry was not available). Then I drew a construction line as close to the axis of the Main Dowel as I could and revolved the Pulley sketch around it. The result is good enough for my purposes, but not really "correct" in my view.

4. Main Dowel is construed by the program to be in three pieces. If you click on it only the section you click on gets selected. This has not caused a problem but I wondered why since the piece was padded into place form a single sketch.

5. To put the two cross braces into place I first created a slab between the uprights and then pocketed the middle part of it to leave the two braces. I had to draw the sketch for the slab on the bottom of the base plate and then pad up through it into the space between the uprights. I could not make the drawing on the top of the base plate because, when I selected that surface to sketch on, the view down onto it was blocked by the Main Dowel and Pulley. I could make the Pulley invisible but, when I toggled the visibility of the Main Dowel, the whole structure, including the base plate, became invisible. I got around it as I explained, but, in general, how do you get an unobstructed view of an surface behind another element of the drawing?

You (and others) have been very kind to give me help, advice and explanations and I thank you very much.

Jim

[chrisb]

You should install the graphviz package so you can use Menubar->Tools->Dependency graph. It looks like this:

Bildschirmfoto 2017-03-16 um 00.02.11.png (36.13 KiB) Viewed 1470 times

and it shows, that you have forked your model: Until Uprights the graph is a straight line, then you attached Sketch002 to a face and made pocket Right Slot. Then you placed Sketch003 and pocketed Left Slot. That was still ok.
But here comes the error: You made somehow Uprights visible again and you attached Sketch004.
You can repair the model by means of Reorientation and attach face:

- Select Sketch004
- Menu->PartDesign->Reorient Sketch, Say yes to detach from Support and Cancel to the reorientation dialog.
- detach in the same way Sketch005
- Now make sure you have only Left Slot visible!!!
- Select the face where you want to attach the Sketch004 for Main Dowel
- Menu->PartDesign->Map Sketch to face (there is an icon too for direct access) and select Sketch004.
- Yo have lost the connection to the external geometry, reinstall it and close the sketch

Now Main Dowel and Right Dowel are in the right place, make Right Dowel visible and DON't FORGET TO MAKE Left Slot INVISIBLE.

Continue in the same way with the other sketches. You have a minor problem: the sequence in the tree does not reflect the dependencies any more. You can repair this by greating a group and moving the pads and pockets in the sequence of your desire into that group.

I attach the model in the state described here.