tangential von Bogen zu Bogen
FeaturedHallo,
wie kann ich in DesignSpark Mechanical untenstehende Zeichnung verwirklichen. Ich einiges probiert und auch gesucht, aber keine Lösung gefunden.
Viele dank schon im Voraus
Gruss skater57

Draw 'Construction' lines from the measurements, shown in 'Green' Draw circles on the 'Intersections' shown in 'Red' Draw '3 Point Circles' and lines tangent to circles, shown in 'Blue'
Delete 'Construction lines' Trim all other lines.
Zeichnen Sie 'Konstruktions'Linien aus den Maßen, die in' Grün 'angezeigt werden. Zeichnen Sie Kreise auf den' Schnittpunkten ', die in' Rot 'angezeigt werden. Zeichnen Sie' 3PunktKreise 'und tangentiale Linien zu Kreisen, die in' Blau 'angezeigt werden.
'Konstruktionslinien löschen' Alle anderen Linien kürzen.
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Hallo, wie Jacant gezeigt hat, ist dies eine Lektion in fortgeschrittener 2DGeometrie der alten Schule. Ein Verständnis der richtigen und genauen Bemaßung, das nur auf eine Weise interpretiert werden kann und keine Mehrdeutigkeit zulässt.
Es ist eine komplexe Form. Die Bemaßung ermöglicht eine gewisse parametrische Änderung.Hello, as Jacant has shown, this is a lesson in 'old school' advanced 2D geometry. An understanding of proper and exact dimensioning that can only interpret in one way only, allowing zero ambiquiety.
It is a complex shape. The way it has been dimensioned allows for some parametric modification.0 
Hi Me Here,
I thought i'd give it a go... ( too much spare time on my hands...)
I, like you, find the junction/ meeting/ point of coincidence between R138 and R288 not easy , nor obvious and i agree with your arc tangent tool comments
Outlining the procedure here is for others not familiar with 2D methods of construction.
The position of R288 is defined by given dimensions 288 , R12, 200, 95 and 255. The center of R288 is found by offseting R12 and furthermost LH vertical end.
The position of R138 is defined by given dimensions 95,105, R15 and the center of R288 as above. At R288 center, make construct circle of rad 150 ( the difference between R288  R138 ) and a construct circle of R123 from R15 arc center ( to make138). The construct circles intersect at 2 places, one of these is the center of a perfect tangential arc between R15 and R288.
So the problem here (?) is with the way it has been dimensioned  previously, a 'draughtsman' would have determined the dimensioning methodology, to depict the part unambiguiosly and clearly for manufacture/ inspection etc , now we have algorithms that quickly determine information 'completeness' rather than helpfulness...all a bit less interesting really but , i shouldn't forget the CAE revolution of commonplace FEM capabilities that's making designing real intellectual fun :).
Cheers  Happy New Year
Tim
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Sorry not the arc tool but the 3point circle tool
Draw all of the 'Construction' lines shown in green.
Draw known positions of circles shown red.
Draw the 576Ø circle using the 3 Point circle tool. Use the 'Tangent' of the 24Ø circle the 'Tangent' of the vertical green line and the third point is the 'Dimension' of the 576Ø typed in. (288*2)
The same for the 276Ø circle. Use the 'Tangent' of the 30Ø circle and the 'Tangent' of 576Ø circle just drawn. With the last point being the 'Dimension' of 276Ø typed in. (138*2)
Trim to suit.
Using the same method for the R178 and R167 Arcs. use the 'Tangents' of the known circles and type in the 'Dimension' for the last point.
The R40 Arc can be found by placing a circle at the center of the 120Ø circle with the Diameter of 200 (120+80)
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Jacant,
Geez, that's so simply compared to my 'longhand' method  works beautifully...
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The command line in AutoCad was known as TTR. Tangent, Tangent, Radius. That's how I knew how to do it. I was trained on AutoCad in the days of Windows 3.1 and MSDos.
Hope everyone is familiar with this now.
If you are interested I will upload a few drawings for you to peruse and practise on.
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Hello Me here  ummn, me here to , exactly as you say , sometimes it doesn't compute correctly  with the R288 i had an identical situation...i have discovered that if you again select the wacko number and enter again it always corrects itself perfectly.
I've been trying various different combo's of everything imaginable by selecting two circles ( tangent edge) and entering a a diameter or 2x R etc and just when it fails twice in a particular method, the third time it works perfectly...
Here's my best effort  i'll be reporting a bug with these results.
Selecting two circles. then move cursor around producing an inflexion as the curve stretches to infinity then into an opposite curve ( easy to do ), then back again to approx desired position, now hit space bar entering a round number, Results as below over 7 sequential inputs.
Cursor box Enter amount Result
300.13 300 300
263.379 263 262.988
353.65 350 349.984
514.453 515 515
319.043 320 319.984
188.941 180 179.966
202.057 200 199.926
As i said though, select wacko result and re enter value does correct it.
The correct inputting method is to always click ( select) a third input position before either hitting the space bar ( or not as still possible ?!) and then entering desired value  so far worked everytime.
I will still raise it as a bug though !
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'But the fun is going out of it now' Yeah, gotcha, but it's just another modelling challenge to overcome and as a 'job' it has to be done. But for 'fun and enjoyment' and interest there has to be sensible limits...
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As Tim has suggested type the number, If it is wrong select the value and input the correct value.
Don't forget any of the dimensions can be changed even after you have made the model into a solid.
Copy and Paste the top surface. Hide Solid. Make new Sketch plane. Select any curve and change to suit.
Not exactly 'Parametric' because the solid will not be updated. Just create a new solid from this sketch.
The inconsistent ones can still be changed because the 'Maintain Sketch Connectivity' will still apply so all tangents will be kept.
Of course you can still 'Pull' the curves in 3D mode to the correct sizes.
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