Sketches, part design, and workflow questions

[revolt_randy]

Hi all,

A question about workflow in FreeCAD. I've created a sketch of a part:

Screenshot2.png (176.47 KiB) Viewed 1696 times

Now I need to add 9 holes to this part, what's the best way to do this? Create all 9 holes in the sketch, cluttering that view? Or create 9 cylinders in Part workbench and boolean out the holes? Or is there a better way to add holes to my part?

Thanks,
Randy

[quick61]

Hi all,

A question about workflow in FreeCAD. I've created a sketch of a part:

[snip image]

Now I need to add 9 holes to this part, what's the best way to do this? Create all 9 holes in the sketch, cluttering that view? Or create 9 cylinders in Part workbench and boolean out the holes? Or is there a better way to add holes to my part?

Thanks,
Randy

What I would do would be to stop there with that sketch and Pad it to the desired height. Then make a new sketch with he holes. If any of them are in a pattern, make one set of then and polar pattern the rest around. Like in the example below -

motormount1.png (14.58 KiB) Viewed 1690 times

And the file -

motormount.fcstd

(31.79 KiB) Downloaded 29 times

Ill also add that your sketch in the snapshot seems to be making good use of the distance constraints. While this works, it is not the most desirable way to go about it. If you haven't see it, I made a post with a little micro lesson on using constraints here - viewtopic.php?f=3&t=11170#p89843

Here is your sketch constrained a better way. Notice I'm using a few less distance constraints.

motormount2.png (22.22 KiB) Viewed 1690 times

Mark

OS: Kubuntu 14.04.2 LTS
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.16.5155 (Git)
Build type: Release
Branch: master
Hash: 882ecd3ce3d7fd7867ac1ef8346308b082d33a92
Python version: 2.7.6
Qt version: 4.8.6
Coin version: 4.0.0a
OCC version: 6.8.0.oce-0.17

[Jee-Bee]

I think the most fast method is create on cut and create a multi transform with first linear pattern and after that polar pattern.

[revolt_randy]

Thanks for the replies!!!

I hadn't thought about using other sketches to create holes, sounds like this is the best way! So far, all other holes I've made in padded sketches I've done with a cylinder and boolean in part workbench. Seems like I can be much more precise using sketches & constraints than just eye-balling the placement of a cylinder.

I downloaded quick61's file and looked at it. It all makes sense to me and I can delete pockets and re-add those pockets back in, When I tried that in my project, I got an error:

Screenshot3.png (136.21 KiB) Viewed 1647 times

At first, thought it was maybe because my sketch wasn't on the surface of the padded part, even though that's not what the error message is telling me.

Can someone describe this error or point me to the docs on this? And what am I doing wrong?

As I'm learning FreeCAD, I'm impressed by it's abilities.

Thanks,
Randy

ps - attached my file

[quick61]

Your sketch is not associated with the part, or in other words the sketch is not mapped to the face. To make a new sketch for a part, select the face you want the feature to be added and click it. In this case that would be the top and then select new sketch. This will map the sketch to that face and become a feature of that part. If the sketch so not mapped to the face and you wish it to be, click the face, then click on the Map sketch to face button and pick the sketch out of the pulldown list. Now, once a sketch is mapped to the face, you can close it and select pocket to make the hole.

Mark

[revolt_randy]

Thanks for the tip Mark! I now have my part designed. I read your micro lesson about constraints and I get what you are saying, best to use relational constraints over distance constraints. This will make modifying the part later much easier. I shall spend some time studying the wiki & searching for constraint tutorials.

So now that I got this down, I revisited an older sketch that I created. I need 6 holes in it, 2 down the center line, 2 on a straight line 120 degrees from center line, and 2 on a straight line -120 degrees from center. Created a center line, & 2 circles, positioned with constraints, then tried to pocket the sketch and it failed. Figured out I had to remove the center line to get it to work. Seems counter productive, is there a better way to position 2 holes along a straight line without creating the line & deleting it?

Thanks for the help!
Randy

[bejant]

Created a center line, & 2 circles, positioned with constraints, then tried to pocket the sketch and it failed. Figured out I had to remove the center line to get it to work. Seems counter productive, is there a better way to position 2 holes along a straight line without creating the line & deleting it?

Yes, in Sketcher try changing those lines to Construction Geometry (blue color) by using this tool:

[revolt_randy]

Yes, construction lines did the trick. I found out about them after my last post.

up next, what is the best way to handle something like this?

side view:

screenshot.5.jpg (248.91 KiB) Viewed 1412 times

front view:

screenshot.6.jpg (245.02 KiB) Viewed 1412 times

I used 2 sketches, a front and a side view, padded each till they intersected, then used the boolean tool on them set to intersection. Is there a better way to do this? Or am I on the right track?

Up next, I have to add holes to both this part and another part, what;s the best way to do that? create one sketch and copy it, assigning the copy to another face?

Thanks much for the help. having fun with this software!

Randy

[revolt_randy]

Right, so used sketches, pads, & pockets and what not. The model is finished and now I move to the drawing workbench, to get blueprints of my parts.

Here's my model:

Screenshot4.png (163.83 KiB) Viewed 1376 times

In drawing workbench, I ad views of my part:

Screenshot5.png (198.6 KiB) Viewed 1376 times

Since the arm isn't square in the top view, (by square, I mean at 90 deg angles) it shows up in the drawing as an angled part. Is there anyway to change this? How to make this part square in the drawing workbench?

thanks for the help,
Randy

[microelly2]

Create a Draft Clone of your part
The clone can be placed free in space
the workfeature macros and the fccamera macro too will support you to align it.
then create the drawing of the clone.