Is Contextual Design Possible without the Assembly WB?

[Sage Brush]

The idea is, let's say I have two parts. I want to bolt them together but don't know where to put the bolt holes. Is it possible to put the parts into a file, and then "drill" the bolt holes in the correct places? I have a few ideas but am not sure what to try:

1) Import the parts into a new file, as STEP files. Align the parts. Create a cylinder and place it where I want a hole to be. Measure from some convenient place on each part to the cylinder. Use the measurements to put holes in the corresponding places on each part, in their respective files.

2) Create two separate parts using the Part WB. (This will make for a rather messy dependency tree.) Align the parts. Put a cylinder where I want the hole to be in the FIRST part. Subtract the cylinder from that part. Put a second cylinder where I want the same hole to be in the SECOND part. Subtract the second cylinder from the second part. (I think using two cylinders will help keep the dependency tree from becoming cross-branched into madness.)

3) Say the first part has been created with a hole in it already. Open a new file and create the second part using the Part Design WB. Import the first part as a STEP (with it's hole) into the second part's file. Align the parts. Place a sketch with a circle in it where the hole should extend into the second part. Align the circle (how?) and create a pocket (hole) in the second part.

Does anyone have an idea? I'm assuming that I can't somehow get a part to span separate files so that if the second file is changed the first file would be updated? Anyway it seems like a work around might be possible without the yet to be released Assembly WB. Also it occurred to me that method 3 might be handy if I want to use an off-the-shelf part. To transfer holes, all I would have to do is download the STEP file from the manufacturer and import it. The rest would be easy.

Sage Brush

[bejant]

1) ... Import the parts into a new file, as STEP files. Align the parts. Create a cylinder and place it where I want a hole to be. Measure from some convenient place on each part to the cylinder. Use the measurements to put holes in the corresponding places on each part, in their respective files.

You can directly use the cylinder to create the hole by using a boolean difference (Part WB) to subtract it from the other shapes.

2) ... Put a cylinder where I want the hole to be in the FIRST part. Subtract the cylinder from that part. Put a second cylinder where I want the same hole to be in the SECOND part

You can use the same cylinder twice.

[Sage Brush]

Hi bejant.

You can directly use the cylinder to create the hole by using a boolean difference (Part WB) to subtract it from the other shapes.

I see, yes you could do a boolean difference on the STEP parts in method 1. One concern I have is that now there are two versions of the same part, one with a full feature tree and the STEP one with the new hole. Hence my idea of putting the holes in the original parts.

You can use the same cylinder twice.

Hmm. That won't make other operations fail later? Then again, the whole idea in method 2 will make a mess.

Do you have an idea how one might align the circle in the sketch in method 3? I can't use Move in the Draft WB to snap the circle to something can I?

Sage Brush

[bejant]

One concern I have is that now there are two versions of the same part, one with a full feature tree and the STEP one with the new hole. Hence my idea of putting the holes in the original parts.

Yes, but you could also do a File > New, then File > Merge Project, and select the .fcstd FreeCAD model, then repeat for the other file. At least now you are working with two .fsctd files that retain their parametric history, instead of "dumb" non-parametric .step files. But when you modify both items by putting a hole in each, they're different than the files you merged. This could be either good or bad...

Hmm. That won't make other operations fail later?

No, here the same cylinder was used to create two separate holes:

20141022a_Sage_Brush.png (18.08 KiB) Viewed 1642 times

The file is attached if you'd like to have a look.

But that causes both items to be dependent on the cylinder. It may be a good thing though (you'll have to decide) because if the cylinder diameter changes, the holes update too:

20141022b_Sage_Brush.png (27.17 KiB) Viewed 1642 times

Do you have an idea how one might align the circle in the sketch in method 3? I can't use Move in the Draft WB to snap the circle to something can I?

3) Say the first part has been created with a hole in it already. Open a new file and create the second part using the Part Design WB. Import the first part as a STEP (with it's hole) into the second part's file. Align the parts. Place a sketch with a circle in it where the hole should extend into the second part. Align the circle (how?) and create a pocket (hole) in the second part

I would merge the first part instead of importing it as a .step file. Then after you align the parts, you can create a Sketch on the first part, use the Link To External Geometry tool

to make a new circle the exact diameter of the hole on it. Now use Pad to fill in the hole, and go through the second part. Now boolean difference the first part from the second to create the hole.

To align the circles you can also use the X,Y, Z coordinates of the circle center, or the alignment tool. Here are some relevant videos that show these methods:
http://www.youtube.com/watch?v=YnbjOlpGGzI
http://www.youtube.com/watch?v=lfinO3EGXeo

[jmaustpc]

Its a bit complex to use, but you can read and set (and control) values with the spreadsheet work bench.

[Sage Brush]

Hmm. I knew there were ways of doing this I had not thought of. Thank you for the replies. I did a little experimenting last night before reading these replies and sort of got things to work by subtracting a set of cylinders from both parts. (I've attached the file below.) Here my ignorance starts to show. I simply made both parts in the Part WB and then selected the top feature of the 1st part and aligned it with the 2nd part. It works but I assume that's not the right way to move a part. In another file (not attached), I remade the 1st part so that I could simply select the first sketch and move that. But since the 1st part is made using the Revolve tool (which seems to be based on the file's origin) the revolved features break when I move the first sketch. Does one have to carefully create a part that does not have any features that could break when the part is moved?

I had not thought of using File > Merge Project at all. I'll try that next time.

I would merge the first part instead of importing it as a .step file. Then after you align the parts, you can create a Sketch on the first part, use the Link To External Geometry tool to make a new circle the exact diameter of the hole on it. Now use Pad to fill in the hole, and go through the second part. Now boolean difference the first part from the second to create the hole.

Ah. That would work better.

To align the circles you can also use the X,Y, Z coordinates of the circle center, or the alignment tool.

Its a bit complex to use, but you can read and set (and control) values with the spreadsheet work bench.

I'll have to look into these things too. I have used the Alignment tool some but not much.

Sage Brush

[bejant]

Does one have to carefully create a part that does not have any features that could break when the part is moved?

No, you can use Draft WB > Clone:

and then move the Clone.

Here I edited the Sketch "2nd_part" to make it bigger, made a Clone of your HolePattern001, moved it Y = -300mm, and subtracted the clone from your 2nd_part to make another set of holes:

20141024a.png (11.48 KiB) Viewed 1572 times

The result is that if you change the hole radius in the Sketch "Hole_Pattern" from 5mm to 10mm, all the cylinders and bolt holes update too.

For example, you can make a Clone of 1st_Part, reorient it, and if any geometry in 1st_Part changes, the clone updates too.

Just a tip:
If you make a Sketch in the Part Design WB, you probably should get in the habit of using Part Design WB Pad:

to create a solid instead of changing to the Part WB and using Extrude.