Sketch is offset by small amount

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TheMarkster
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Re: Sketch is offset by small amount

Post by TheMarkster »

dcschooley wrote: Tue Jan 18, 2022 8:01 pm
The rotation was caused when I changed a pad or something and it rotated the sketch. I tried to fix it by rotating it somewhere else. I tend to tweak my designs a lot, so that topological naming problem causes all sorts of havoc. I am going to redo this drawing from scratch using datum planes to see if that helps.
Attaching a datum plane to the same face and then attaching a sketch to that datum plane is akin to climbing into a sinking ship and expecting not to drown.
dcschooley
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Re: Sketch is offset by small amount

Post by dcschooley »

I redid the part using datum planes instead of attaching sketches to pads. Everything worked much, much better. I was also able to mirror the padded block with the screw holes, so I didn't have to try to duplicate that sketch. I even experimented with deleting most of the pads and all of the pockets and everything still worked. I still ran into one problem where fillets applied before the last two pockets kept the pockets from showing up in the exported stl. Doing the fillets at the end fixed the problem.

Thank you everyone for responding. The suggestion about mirroring was an enormous help.
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drmacro
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Re: Sketch is offset by small amount

Post by drmacro »

dcschooley wrote: Wed Jan 19, 2022 1:41 am I redid the part using datum planes instead of attaching sketches to pads. Everything worked much, much better. I was also able to mirror the padded block with the screw holes, so I didn't have to try to duplicate that sketch. I even experimented with deleting most of the pads and all of the pockets and everything still worked. I still ran into one problem where fillets applied before the last two pockets kept the pockets from showing up in the exported stl. Doing the fillets at the end fixed the problem.

Thank you everyone for responding. The suggestion about mirroring was an enormous help.
I'm not at PC, so can't check the file. But if you attached the datums to faces, then you have not made the most robust model. If the datums are instead attached to base planes then you have succeeded in improving the stability.

Fillets are always a possible source of issues because of TNP and limitations in the modeling kernel.
Star Trek II: The Wrath of Khan: Spock: "...His pattern indicates two-dimensional thinking."
chrisb
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Re: Sketch is offset by small amount

Post by chrisb »

The DatumPlanes are all constructed in a stable way. However, if you attach only a single sketch to them, then it is no gain to have the DatumPlane, you could use the same attachment directly in the sketch.
A Sketcher Lecture with in-depth information is available in English, auf Deutsch, en français, en español.
dcschooley
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Re: Sketch is offset by small amount

Post by dcschooley »

chrisb wrote: Wed Jan 19, 2022 1:00 pm The DatumPlanes are all constructed in a stable way. However, if you attach only a single sketch to them, then it is no gain to have the DatumPlane, you could use the same attachment directly in the sketch.
So in other words, where in one case where the DatumPlane is simply raised 2mm from the origin X-Y plane, I could have attached the sketch to the origin X-Y plane and raised it by 2mm? That makes sense.

It's amazing how much more stable the model is.
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Re: Sketch is offset by small amount

Post by chrisb »

dcschooley wrote: Wed Jan 19, 2022 1:47 pm It's amazing how much more stable the model is.
Yes, it's becoming fun! There is a good Basic Attachment Tutorial explaining the power of attachments.
A Sketcher Lecture with in-depth information is available in English, auf Deutsch, en français, en español.
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Shalmeneser
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Re: Sketch is offset by small amount

Post by Shalmeneser »

Your sketches are too complex.
So it's impossible to use Sketcher_External because too much things can happen.

* 11 = 22/2 : use Sketcher_ConstrainSymmetric
* 3 and R1 : not logic
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dcschooley
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Re: Sketch is offset by small amount

Post by dcschooley »

chrisb wrote: Wed Jan 19, 2022 5:09 pm
dcschooley wrote: Wed Jan 19, 2022 1:47 pm It's amazing how much more stable the model is.
Yes, it's becoming fun! There is a good Basic Attachment Tutorial explaining the power of attachments.
The main reason I've given up on FreeCAD a couple of times in the past is that my drawings were never stable because I was always attaching sketches to faces of pads or whatever. I would spend so much time trying to fix stuff after it got messed up that it just wasn't worth the bother. Between now knowing what I was doing wrong wrt attaching sketches to things and realizing that I can put data into a spreadsheet, life should be much better.
dcschooley
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Re: Sketch is offset by small amount

Post by dcschooley »

Shalmeneser wrote: Wed Jan 19, 2022 5:26 pm Your sketches are too complex.
So it's impossible to use Sketcher_External because too much things can happen.

* 11 = 22/2 : use Sketcher_ConstrainSymmetric
* 3 and R1 : not logic
Thanks! I've been using equality constraints. Being able to use symmetry will be helpful.

What do you not like about the 3 and R1? The 3mm was the original spacing and then I added the fillet later.
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Shalmeneser
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Re: Sketch is offset by small amount

Post by Shalmeneser »

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Capture du 2022-01-19 19-36-24.png
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