Alignment Question

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h.dale
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Alignment Question

Postby h.dale » Thu Dec 25, 2014 7:12 pm

I am trying to use FreeCad to create a drawing for parts to a fuselage similar to the one shown below. I can create the parts but I need to cut a hole through all of them at the same time so I can put an alignment rod through them. Could someone show me how to do this?

Thanks for any help.

Hal
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quick61
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Re: Alignment Question

Postby quick61 » Thu Dec 25, 2014 8:08 pm

Hi Hal,

What you need to do is select all your formers once you have them positioned where you want them in 3D space and use Part > Make compound. This will make a compound of all the formers. Then it is a simple matter of placing a Cylinder where you wish the holes to be for your alignment pin to pass through and then Cut the Cylinedr from the compound.
Alignment_Hole.png
Alignment_Hole.png (61.08 KiB) Viewed 1993 times
Let me know if this helps or if you might wish further clarification.

Mark
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h.dale
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Re: Alignment Question

Postby h.dale » Thu Dec 25, 2014 8:31 pm

Thanks Mark. That was simple enough.

Hope you had and Merry Christmas and have a happy new year.
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quick61
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Re: Alignment Question

Postby quick61 » Thu Dec 25, 2014 9:41 pm

h.dale wrote:Thanks Mark. That was simple enough.

Hope you had and Merry Christmas and have a happy new year.
Your welcome and back at ya. :)
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quick61
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Re: Alignment Question

Postby quick61 » Thu Dec 25, 2014 10:16 pm

Thinking about this, what I told you only get's you half way there, if your intending to take this into the real world.

What you will end up needing is either a set of templates or something for tool paths to cut the parts out. What I would do from this point, once all the alignment holes and such were Cut into the former assembly, would be to use the Part > Create simple copy tool and make a simple copy of the final former set. I would then copy that simple copy into a new document (you can now delete the simple copy from your original document), and open the Draft Workbench. Select the simple copy in your new document and use the Draft > Downgrade tool on it. This will explode your simple copy into a group of solids that should be your individual formers with the hole(s) in their proper location. Now, for each solid, select it and create a 2DShapeView for each one. From this point, you can select your 2DShapeViews and using the Draft > Move tool, place them in whatever order you wish to make your templates or for DXF/SVG export for your CAM package if your CNCing the parts out with laser or router.
Alignment_Hole1.png
Example of 2DShapeViews placed for tool path or templates.
Alignment_Hole1.png (24.28 KiB) Viewed 1962 times
Mark
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h.dale
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Re: Alignment Question

Postby h.dale » Fri Dec 26, 2014 4:52 pm

Mark

I have tried your method with a sample file and I think I have done something wrong. I created two circles, made them a compound but when I try to map to the face of the smaller one to cut the hole it maps to the back side and I can't see it. I've attached the file. Where have I gone wrong?

Hal
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quick61
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Re: Alignment Question

Postby quick61 » Fri Dec 26, 2014 5:22 pm

h.dale wrote:Mark

I have tried your method with a sample file and I think I have done something wrong. I created two circles, made them a compound but when I try to map to the face of the smaller one to cut the hole it maps to the back side and I can't see it. I've attached the file. Where have I gone wrong?

Hal
By trying to use Part Design for this operation...

I should of been more clear on that point, sorry. You need to use the Part Workbench and it's Boolean operations. Use Part > Cylinder or whatever shape you need, (could even be an extrude from a Draft object or Sketch) and do a Boolean Difference, AKA Cut, of the shape from the compound. Part Design Features do not play well with Compounds, as you have discovered.
mig_29a.fcstd
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Mark
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h.dale
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Re: Alignment Question

Postby h.dale » Fri Dec 26, 2014 5:58 pm

Thanks Mark.

I'm rocking and rolling now.

Hal
h.dale
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Re: Alignment Question

Postby h.dale » Sat Dec 27, 2014 4:57 pm

Mark

I have another question. The photos above show a stringer that runs along the top and bottom of the fuselage. How would you create the stringer and move it into place? I was thinking I could use a side view of the plane, draw and pad the part and then move it into place and do a cut. Will that work?

Can you select a part and move it with your mouse or do have to move it by changing the data in the data tab?

Thanks.

Hal
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quick61
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Re: Alignment Question

Postby quick61 » Sat Dec 27, 2014 5:22 pm

h.dale wrote:Mark

I have another question. The photos above show a stringer that runs along the top and bottom of the fuselage. How would you create the stringer move it into place? I was thinking I could use a side view of the plane, draw and pad the part and then move it into place and do a cut. Will that work?

Can you select a part move it with your mouse or do have to move by changing the data in the data tab?

Thanks.

Hal
You can move parts with the mouse using the Draft > Move tool. There are a few things to note when doing so. First is, if you use a Sketch and Pad, moving that part can only be done by selecting the Sketch and moving it to place the part, so doing a mouse move snapping a center line to another center line takes thought when making your Pad as you will be snapping the Sketch, not the part. in this case you would use the Symmetric to plane opting in the Pad dialog. I personally think that using either a simple copy or Draft > Clone for parts made from Sketches that I will be moving is a good option. Make your Sketch and Pad it to create the stringer then make a Draft > Clone or Simple copy of that part and then use the Draft > Move tool with ONLY the desired snapping action turned on. only have 1 or 3 snap options turned on at most or you will start to run into problems. The Passive snap will really give you fits so don't use it until you have a good grasp on FreeCAD's Draft > Snap workings.

Another option would be to use a Sketch or Draft object to define the spline profile and lay out a path for it and do a Part > Sweep. This is a good option if you have a lot of bends and curves involved with your stringer or any such feature of your assembly.

Mark

Edit - if you haven't seen it yet, here is a video on Placing Parts in FreeCAD
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