putting sketch perpendicular to another

[FC-Architecter]

OS: Linux Mint 18.3 Sylvia
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.17.13528 (Git)
Build type: None
Branch: releases/FreeCAD-0-17
Hash: 5c3f7bf8ec51e2c7187789f7edba71a7aa82a88b
Python version: 2.7.12
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 7.3.0
Locale: English/UnitedStates (en_US)


I am trying to make an arc with a circle attached to the end point and perpendicular to the arc at the the end.

I will then make a sweep up the arc to create a curved tube.

I will also need to create a sketch and additional features at the far end of the arc. But I think the sweep itself will create a flat disk surface at the far end that I can then attach a sketch of another circle to, and then modify.

So I think it may only be necessary to create the perpendular circle sketch once.

So far I have tried keeping the arc sketch visible when I create the circle sketch, but the arc only shows as a flat line with the endpoints hard to pointpoint so I can't attach the circle precisely.

I can locate the circle sketch001 to the endpoint of the arc if I put a point-to-line constraint on the arc to one of the axes. I tried attaching

Any assistance appreciated.

arc.png (6.68 KiB) Viewed 2085 times

Here I attached the circle to the arc endpoint by eyeballing it. I don't think that is a precise method.

EYEBALLING_CIRCLE_AND_ARC.png (2.94 KiB) Viewed 2078 times

[salp]

The two sketched do not need to be attached, I used Parts Design workbench.
See the attached file.

Screenshot from 2018-08-03 20-47-37.png (98.42 KiB) Viewed 2079 times

SweepExample.fcstd

(9.26 KiB) Downloaded 44 times

OS: Linux Mint 18.2 Sonya
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.18.14183 (Git)
Build type: None
Branch: master
Hash: 8ef330d19ab4aa0cfd6b9a6d41d51eed30620707
Python version: 2.7.12
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 7.3.0
Locale: English/UnitedStates (en_US)

[FC-Architecter]

The two sketched do not need to be attached, I used Parts Design workbench.
See the attached file.
....

Thanks for responding.

I am not very good at analysing other people's files. But I don't see a feature called sweep. So I cannot tell if Frenet was used. Frenet affects how the sweep turns at is moves up the path, right?

How do you know your pipe is precise if you need to use it for industrial purposes?

[salp]

It looks like you are using the Parts workbench, I'm not familiar with that.

I used the Parts Design workbench, the 4th icon down the right side of the screen shot.

The Way I use it is to hold down the CTRL key and select both sketches, that in the selection window click on the "Object" button then click on sweep path.


To ensure it's precise you need to constrain both sketches (radius and arc length of the curve, and the radius of the circle), I also use the Tech Draw workbenches and display the dimensions just to make sure.

Hope this helps.
Sal

[meme2704]

Hi
I think you want to build a "real" pipe of constant circular section
you must place the sketch of the circle representing the section, and the path representing the curve, rigorously perpendicular to the origin.
So place first (it's not mandatory but it's better when you start) the circle section, in the XY plane for example, constrains the diameter and position OX and OY
In a perpendicular plane XZ for example, place the arc for the path, choose the center point of the curve. it is not necessary to specify the radius of the arc path, only its angle is important
you do the sweep that will be coming from the circle section
Then you use placement to place it in the right angle, and in the right place
This is done with the workshop "Part
With PartDesign, some will offer you the entire gas plant

[mario52]

hi

try this macro Macro_Perpendicular_To_Wire

example arc and circle



EDIT:06-08-2018 20h35 Paris
replace image with appropriate example

mario

[FC-Architecter]

....
you must place the sketch of the circle representing the section, and the path representing the curve, rigorously perpendicular to the origin.
So place first (it's not mandatory but it's better when you start) the circle section, in the XY plane for example, constrains the diameter and position OX and OY
In a perpendicular plane XZ for example, place the arc for the path, choose the center point of the curve. it is not necessary to specify the radius of the arc path, only its angle is important
you do the sweep that will be coming from the circle section
Then you use placement to place it in the right angle, and in the right place
This is done with the workshop "Part
With PartDesign, some will offer you the entire gas plant

Thanks for responding.
1) I think you mean to make the circle before the arc. The circle should be in the XY plane.

2) then make the arc in the XZ plane.

It seems like using placement is just eyeballing it. Unless you exactly how far the circle center is from the arc end-point in millimeters. If both circle and arc are made starting on the origin but in different planes, that might work.

Maybe that is what you meant here?:"So place first (it's not mandatory but it's better when you start) the circle section, in the XY plane for example, constrains the diameter and position OX and OY"

Otherwise. after 1 and 2 have been done, is there a way to use the point coincidence constraint to join the center of the circle to the end-point of the arc?

I don't quite get the "gas plant" reference.

[microelly2]

If you have created the first sketch onto a datum plane
you can create a new datum plane for the 2nd sketch which is perpendicular to the first
You define an attachment condition Objects XZ or YZ

bp_867.png (60.33 KiB) Viewed 1970 times

There is another way possible too:
define the attachment by 3 points and use MapMode O-X-N

[meme2704]

I meant that if you want to have a pipe of circular section, it is necessary that the tangent to the starting point of the path must be perpendicular to the plane of the section, whatever the position of the path in the space.
"gas plant" is a Franco-French expression for a complex pipe array

[FC-Architecter]

If you have created the first sketch onto a datum plane
you can create a new datum plane for the 2nd sketch which is perpendicular to the first
You define an attachment condition Objects XZ or YZ
bp_867.png
There is another way possible too:
define the attachment by 3 points and use MapMode O-X-N

Thanks for showing how to use the datum plane for this. I just learned about the datum plane in the wiki tutorials.