Merge sketches and other questions

[Troymx576]

If I understand what you are trying to do you just need to modify the z attachment offset of Sketch006 to something like z = -3mm.

Snip macro screenshot-359055.png

Note: it is not recommended to attach sketches to faces due to some issues it can cause if you decide later to modify some of the earlier sketches. If things go crazy you just need to go back in and reattach the sketches to the correct faces (usually anyway).

That is exactly what I was wanting. I was trying to move the pocket location and not the sketch location.

Now I have another issue on it. I want to go in and change the Y position to zero and move the Z position and they highlight, but I can not do anything with it as it is frozen or locked. How do I make it editable?

Thank you
Troy

edit- Also, when I click in the area and try to type numbers it flips the view of the object around.

[GeneFC]

There are two places in the property panel where it appears you can change the z-offset. Only one of them will work in most situations.

One place is in the "Base" property heading (does not work here) and the other is in the "Attachment" property heading (works).

This can be confusing at times, and even after thousands of attemps I sometimes try the wrong one first.

The other thing to mention is that "Combo" panel includes both the "Tree" and the "Property" panels. You will have more room in the left column if you turn off the "Tree" panel and just keep the "Combo" panel.

Gene

[TheMarkster]

Part Design features, such as pockets, do not have placement properties and must be moved by moving the sketch used to create them. An attached sketch will have 2 placement type properties: the placement property and the attachment offset property. (An unattached sketch only has the placement property visible.) For an attached sketch its placement property is read only and is calculated by FreeCAD based on the position of the object to which it is attached and on the attachment offset property. (But it's actual position in global space is determined also by the placement of its Body container in Part Design and/or its parent Part container's placement.) Because this placement property is calculated for attached sketches it makes no sense to allow the user to modify it directly, instead the way to do it is to modify the attachment offset property or to move the object to which it is attached or perhaps to modify the attachment mode, e.g. concentric versus inertial cs.

[Troymx576]

There are two places in the property panel where it appears you can change the z-offset. Only one of them will work in most situations.

One place is in the "Base" property heading (does not work here) and the other is in the "Attachment" property heading (works).

This can be confusing at times, and even after thousands of attemps I sometimes try the wrong one first.

The other thing to mention is that "Combo" panel includes both the "Tree" and the "Property" panels. You will have more room in the left column if you turn off the "Tree" panel and just keep the "Combo" panel.

Gene

That did it. I did not even notice the base and attachment, but when using the correct one it worked. I was a bit frustrated knowing it was something simple. Thank you. All is good.

This Freecad is getting to be a lot more fun now that I am able to get to the cad program what is stuck in my mind.

[Troymx576]

I have another noob question.

I started with a basic sketch, pad it. Then on the different faces made more sketches and pad them. I got the part that I want, but having issues putting the needed chamfers where needed and sizes needed. Do I combine it all to make it one part so I can put in chamfers where needed?

In the picture it will only do the chamfer on the small section and when I got to .125 it does not allow it as it goes accross the intersection of the pads.

Also, on the outside you can see all the basic drawing lines there. It prints fine on the 3d printer with STL file and when I go to CNC I would think it would be fine, but if it all looked as one surface or face it would be nicer for the techdrawings.

Thank you yet again.
Troy

[chrisb]

Do I combine it all to make it one part so I can put in chamfers where needed?

Yes, use Part->Union.

Also, on the outside you can see all the basic drawing lines there. It prints fine on the 3d printer with STL file and when I go to CNC I would think it would be fine, but if it all looked as one surface or face it would be nicer for the techdrawings.

Set Refine=true in the last operation, probably the union mentioned above.

[Troymx576]

Do I combine it all to make it one part so I can put in chamfers where needed?

Yes, use Part->Union.

Also, on the outside you can see all the basic drawing lines there. It prints fine on the 3d printer with STL file and when I go to CNC I would think it would be fine, but if it all looked as one surface or face it would be nicer for the techdrawings.

Set Refine=true in the last operation, probably the union mentioned above.

Should I do the boolean union after I add each pad? Or can I do it at the end when it all done? When is the best time? I just tried to do it and it did not fix the portion I am trying to add the larger chamfer to. It also gave me an error that I do not have active face when trying to add the chamfer.

Should I build all the pads in solids first and then fuse each one to one another?

I am looking up boolean tutorials now.

I added and updated FCcad with each part renamed to make it easier to discuss.

[chrisb]

From your last image it looked as if you had several solids, thus the recommendation with the Part->Union. Now I see that it is all done in PartDesign in a single body. So this is something completely different. Not being able to select some edges is probably caused by a graphics card/driver issue. You can up- or downgrade the driver, or try with 0.19, or both, or you leave it as is and use the wireframe display mode for selecting the chamfers.

To get rid of the additional chamfers you can refine the last feature. However, refining doesn't work with holes, so you will have to go back and refine the last pocket "load cell bolt slots".
Alas, you have attached the subsequent sketches to faces, which is not recommended, because it causes exactly what is happening now: The faces have changed their internal numbers and the sketches are mapped to completely different, possibly not even existing faces. So you will have to remap the sketches.
Or you attach e.g. an additional final dummy pad, going only into the existing material and thus not really adding anything. Then you can refine that final pad without breaking the previous steps.

[chrisb]

Concerning the not working refinement on the holes I have created another post.

And I forgot a general remark about your model: You should consider modeling only half of the thing and then mirror it.

[Troymx576]

Concerning the not working refinement on the holes I have created another post.

And I forgot a general remark about your model: You should consider modeling only half of the thing and then mirror it.

I will give that a try. I have not used the mirror function yet and tried that.

I am now trying to figure out how to fuse and union items and even when I just do basic shapes it does not work for me so fundamentally I doing something wrong. Maybe starting in part design and working with sketches to faces like you said. I will some different ways to do it and see what I can come up with.

On the sketch I could go to like .10" chamfer, but not to .125" as it hit the other intersection line.