Help on sketching

[Fron]

Hello! New to this forum, and Freecad.
I have watched some tutorials as long as my patience would go, but I had to give it a shot for myself.!

For 2d drawing I already have a program I feel pretty steady with and I draw the basic shape with measurements there.
Problem came when I was to model the "mounting ears" on the sides of the shape.



Here is what I so far have produced;



So, I am not shure if this is the best way to model these ears. I have read that you should have more sketches than one so I figured is would be best to model the ears for themself in different sketches. But I cant find a decent way to do it, so I would be shure the "ears" models would be mounted exactly at the side of the first sketch/pad and not overlap or causing troubles for later.

As you can see of the first drawing, It should be some reinforcements from the mounting ears to the basepad, this is where it got tricky.
There is a few places here I haven`t set any mesurement, but I hope this shows the problem. Also, I haven`t designed the lower pad where the ears with the reienforcement is accualy going, but this was just to show where it stops for me

Version info:

OS: Windows 10
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.16.6704 (Git)
Build type: Release
Branch: releases/FreeCAD-0-16
Hash: 0c449d7e8f9b2b1fb93e3f8d1865e2f59d7ed253
Python version: 2.7.8
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 6.8.0.oce-0.17

Thanks, Fron:)

[jeno]

Hi Fron,
attached a possible solution for what your after.
Feel free to use it.
cheers
jeno

[quick61]

First thing, there is a problem with your 2D drawing. Your total width is 61.9, but if one adds up the dimensions across the bottom, they come out to be 58. Setting the Arcs at 60* does not allow the distance of 5.1 to exist within the limits of the other dimensions.

Other than that, when placing the ears and their gussets, polar pattern and mirror features are your friend. Model one ear, polar pattern it, then make a small helper pad, (sense you're using 0.16 release), that provides an edge in the middle of the cutout in the ear. Then make a sketch for one side of the gussets and then mirror that with the face from the helper pad that was previously placed in the center of the ear. Now do that for the other side and you should be good to go.

Ears.fcstd

(160.91 KiB) Downloaded 22 times

Mark

OS: Kubuntu 14.04.4 LTS
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.16.6703 (Git)
Build type: Release
Branch: releases/FreeCAD-0-16
Hash: 2ce5c8d2e3020d05005ed71f710e09e9aa561f40
Python version: 2.7.6
Qt version: 4.8.6
Coin version: 4.0.0a
OCC version: 6.8.0.oce-0.18-dev

[Fron]

Wow, seeing the timestamp and considering the sketch took me about 2 hours I guess I have a long way to go.
Will be reading about the tools you wrote, and yes, its exactly what I was planning.

Its a pump for a cooling system, Its a bit in the works, but I figured it would be easier to draw the whole thing 1:1 in 3d, and then do all the pipework and cutting after everything is planned!

By the way; Do you use squares and circles to make "construction" to find the next point or is it easier to calculate your way from the center lines? Haven`t figured this out yet, I am used to just draw in 2d, one layer so you can just continiue on the same block. This mentality does not work as good in 3d, I guess.

Thanks again!
Fron!

[NormandC]

Hello Fron,

I noticed you hosted your images on Imageshack. You can actually upload images to the forum through the Attachments tab below the text box.

Some of us actually prefer images to be hosted here for multiple reasons.

[NormandC]

By the way; Do you use squares and circles to make "construction" to find the next point or is it easier to calculate your way from the center lines? Haven`t figured this out yet

Using the Sketcher to construct your 2D geometry, you hardly ever need to calculate anything.

Maybe if you posted your own FreeCAD document we could have a look at how you made your sketches, and provide advice.

BTW dimensioning fillets with an angular dimension is not the way it's usually done.

[NormandC]

Hey Mark, I think you reversed the position of the ears (Look at his screenshot). The problem is that Fron's ortho views seem to be using First Angle projection. We both know that real technical drawing is done with the Third Angle projection. (J/K!!!)

there is a problem with your 2D drawing. Your total width is 61.9, but if one adds up the dimensions across the bottom, they come out to be 58. Setting the Arcs at 60* does not allow the distance of 5.1 to exist within the limits of the other dimensions.

I think the problem comes from rounding.

Notice there's a 28.05 dimension above. But if you add 5.1+17.95+5.1 you get 28.15. Instead, if you add 4.7+28.05+25.15 then add 4 for the right side chamfer, you do get 61.9 like at the top.

Other than that, when placing the ears and their gussets, polar pattern and mirror features are your friend. Model one ear, polar pattern it, then make a small helper pad

I used to do that a lot, but I've become a little weary of this method which adds a lot of features (since we can only pattern one feature at a time) and tends to weaken the model.

I think here I would model one of the gussets as a separate part like jeno did, create a Draft Array then fuse the array to the main block.

Just goes to show there are always more than one way to get things done in FreeCAD.

[quick61]

Hey Mark, I think you reversed the position of the ears (Look at his screenshot). The problem is that Fron's ortho views seem to be using First Angle projection. We both know that real technical drawing is done with the Third Angle projection. (J/K!!!)

Hokey smokes, your correct. Good 'ol dyslexia kicking in again or some such.

Anyway, I think the model in my post is correct now. Easy fix and only had to redo one sketch that failed.

Mark

[Fron]

Ok.. So I`m this far, left the photo here so you can see where I`m at.

Question; How do i get the "ear" part to connect to the "pumplowerbody" part? Can`t get the "external geometry" tool to find the edges on the "pumplowerbody".

Do I have too many seperate sketches?

About the progress I will have some tubing and a radiator for later when my skills allow it. Should I create them in another file and copy them over to a final file?

Untitled-2.jpg (562.18 KiB) Viewed 1821 times

Thanks,
Fron!

[bejant]

Question; How do i get the "ear" part to connect to the "pumplowerbody" part? Can`t get the "external geometry" tool to find the edges on the "pumplowerbody".

I think that you have two separate solids in your model, the ear and pumplowerbody. Use Tools > Dependency Graph to check that, in Ubuntu it's in the Software Center but I don't know the Kubuntu equivalent to the Software Center.

If you had selected the bottom face of pumplower body and then clicked the Create Sketch button, then SketchEars would have been Mapped onto the bottom face, and you'd have one solid after making a Pad from SketchEars.

You could try using the Map Sketch To Face tool to Map SketchEars onto the bottom face of pumplowerbody, and use the Data tab (lower left corner of the FreeCAD window) change the Reversed property to True if it isn't already.

Or you can select PadEars in the hierarchy tree, from the Data tab change the Reversed property to the opposite of whatever it is now, and in the Part WB use the Boolean Union tool to create a Fusion of pumplowerbody and PadEars.

If that doesn't work, upload your FreeCAD .fcstd file to the forum and someone will troubleshoot it.