Sketch dimensions faulty after redefining the sketch plane

[matti.suuronen]

I have a sketch that is based on a construction plane. The construction plane is defined with "Plane at angle" from an edge in a body. I drew some geometry based on the origin and direction of that plane, but later the body changed, and the origin of the plane decided to move to an arbitrary place (shifted down a few mm as far as I can tell), i.e. it did not coincide with the edge. A new sketch based on the same construction plane did have the origin aligned with the edge, so now had a construction plane that had two different coordinate systems, based of which sketch I was drawing on. That did not seem right. I tried re-defining the construction plane by unselecting the plane-defining edge and selecting it again, but the resulted in the plane being rotated in "x-y" plane so I could no longer use "horizontal/vertical" constraints. While I know  it is _possible_ to draw without vertical/horizontal, it makes thigs more difficult than they need to be. Therefore I redefined the construction against a different edge (at a junction of two 90 degree-angled faces), which resulted in the horizontal/vertical re-aligning (However 90 turned to the right, i.e. XY-plane of the construction plane rotated). So, almost good. However, now on dimension in the sketch seems to act funny, i.e.  a 2mm distance showed initially as something like 11.4763 mm (cannot rememer exactly), even the dimension was indeed 2mm. And now when I change the dimension, the dimension line points to an arbitrary empty spot in the sketch, so I need to remember what it actually refers to. Not nice, but the dimension does work.

The sketch had a projection (points)  from a part of the body, but that seems to have turned into a non-movable point, that does not align with its original part. 
So, is it just me being a noob, or does f360 not play nice with me?

[sutherland-]

Hi @matti.suuronen 

Could you please share the .f3d file here so we can try to reproduce the same behavior that you are facing?

[matti.suuronen]

Sure. Here it is. No laughing at my design 🙂

[sutherland-]

Thanks for sharing!

For the 2mm gap that should be pointing to the tangent circle there are 2 ways to make the circles fully locked/black and so that the dimensions does not go crazy when changing angle of the construction plane.

1. Create a construction line that goes from the midpoint to the circle. Then define the length of the construction line as seen in the screenshot below:

Now when you change the angle of the construction plane, the dimension remains there.

OR

2. I would not suggest to do go this way, but I am just showing it to you so you know how you can play with the dimensions in F360. You could define the distance between the center circle to the point, but then to have the gap dimensions you would need to refer to the circle size. The expression here could be like seen below:

( d130 / 2 ) + 2 mm

where

• d130 is the driven dimension of the bigger circle D 34mm (I got it by pressing the driven dimension number while the input dialog is opened 
• /2 is so that we take the radius of that driven diameter
• +2  is the gap that you want to have

Regarding the random point, I can see that it is locked manually and does not refer to anything. What is it used for? 

[sutherland-]

Here is a GIF for the 2nd point on how to get the dimension inside the input value dialogue.

 

 

[matti.suuronen]

Thanks!

I did have the sketch fully defined, I always define them fully, learned it the hard way a while back :).  For the 2mm distance, I used the "Pick Circle/Arc Target" option for the dimension, as that really is the design intent. And it seems to work most of the time, just now it did not. But your experience/suggestion is that I should not use that option? And centre point is the proper one? (The problem is more or less cosmetic, as the distance is/was kept at 2mm, but the display was rather unorthodox with the wrong value and wrong point it referred to)

The fixed point is now doing nothing. It used to be a projection from a body earlier, and was used to point the construction line to the correct direction. I believe that at some point the reference object vertex got removed, and in the "Manage Lost Projections" dialogs I removed them (not relinked/deleted), and it turned into this unmovable point. Any hints on how I could make sure the projected points are really removed?

[g-andresen]

Hi,

For me, the display error disappeared by editing the plane again.

günther

[sutherland- · Accepted solution]

I would say that there is no "correct" or "incorrect" way of competing the specific task if the outcome is the same. But I do agree that in this situation your way causes weird visual behavior. I will not be able to describe the cause of this, unfortunately.

To delete any projected points you should:

Hold down the left mouse button for around half a second to bring up this menu:

When you move your cursor over this menu, the visuals will cross-highlight to help you pick.

Once you've selected the projected curve, select "Break Link" from the right mouse menu:

But keep in mind that this does exactly what it says. That projected line is no longer associated with the model from which it originated.

Also, one tip - There is a distinct difference between Remove and Delete. 

Remove was once known as a "soft delete." This adds a timeline feature that eliminates this body or component. The body or component will still exist if you travel back in time before using the Remove feature. Delete means "to erase all traces of this item that have ever existed." It is effectively the same as removing the functionality that produced this item in the first place.

[matti.suuronen]

Thanks! Yea, it seems some actions do remove this oddity, so fortunately it is not a permanent thing.

[matti.suuronen]

Right, I was not aware of the difference betwen delete and remove, but it makes sense. Now I am off to erasing those pesky little unintended dots inhabiting my sketches.. Thanks agn for quick help!

[sutherland-]

More than glad that it gave some clarity!
Hope there will be no issues in future, but if there are, do not hesitate to post on forums.