Add Pocket-Hole in Assembly to other Part?

nocry3

I actually have a simple logical question. I have a timber (60×40 cm), which I want to connect by pocket holes with another timber ( 80×80 cm) in an assembly.

If I add a dowel as shown in the picture (left side), it will be displayed in both squared timbers. If I only add a hole for the dowel as in the picture (right side), it is not shown in the other timber.

Is it possible, or how can I make it that a “hole” is displayed depending on the position in the assembly, like the dowel?

https://cad.onshape.com/documents/cdbf4aec9477dbc5258e3d37/w/d1924d7d3a5d07c566f60952/e/ca7472631d213f0223f64370?renderMode=0&uiState=64bd51dc965af537ae385410

nick_papageorge073

If I'm understanding your question, try the following:


Change through all to a blind hole and put in a number that works. On merge scope, select the 80x80 leg, so both parts are in the merge scope. When you are happy with how the dowel hole looks, circular pattern it 90 degrees using the center mate connector of the table leg as the axis.

If instead of a dowel you are using screws, then you might need to split the hole into two features, one for the 60x40, and one for the 80x80, since the diameters are different. But the general procedure would be the same.

glen_dewsbury

Your pocket hole does not merge scope with the 80 x 80 timber. Don't forget to mirror the pocket holes at 45 deg across the 80 x 80.

nocry3

I asked my question a little badly. I have two parts, 60×40 and 80×80. In one part, I can install the pocket holes in the part studio. In the other part 80×80, I can only "install" the holes in the assembly when I know where the 60×40 touches the 80x80.

When I fasten the dowel to the 60×40 pocket hole in the assembly, it also moves in the 80×80 when I fasten it with 60×40 somewhere. If I move the 60×40, for example, 20 cm down, then the dowel is also in the 80×80 20 cm down.

Question: How do I get the same result with the hole inside the 80×80 as with the dowel?

glen_dewsbury

An in context edit of the column sounds like what you need. Once the dowels are located on the column then a Boolean Subtract will work.
If you have multiple locations then you may need to generate part configurations of the column.

nick_papageorge073

I also think in-context edits are what you are asking about, in general.

However in this design, I don't think they are needed. I think you should draw the vertical leg, and the horizontal rails, in the same studio as they would be located in real life (which is what you did). Then put the dowel holes through both pieces in that studio. Then when you switch to the assembly, you can insert the entire part studio, fix one part, and group the rest. There is not really a need to experiment with leg positions for a table. That is well known. And the dowel positions must be within the leg. I just don't see the need for in-context editing in this case.

Or, probably even better, this looks like you are designing a table, correct? Well on a table the main design intent is the size of the top, and the height of the top from the floor. That should be your driving feature. Then there is an inset amount of where the legs attach to the underside of the table. Draw a rectangle sketch as construction lines on the underside of the table, inset from the table edge. Then draw a rectangle representing one leg. Then draw the rails connecting the legs. Now, if the table size changes, the legs and rails will change automatically.

I think there was another member that was making a table a year ago and I might have modeled up what I just described. I'll see if I can find it and link it for you.

nick_papageorge073

Take a look at this studio and assy for some ideas on making a table with a top-down design intent (pun!).

https://cad.onshape.com/documents/c55bd9f097a885f069a96d26/v/02f4b54532a034bbeba18b6d/e/d4875b3cfe46ed30ebd578f7

nocry3

nick_papageorge073 said:

...
Or, probably even better, this looks like you are designing a table, correct?

...

It is a workbench (everything named in German) and I try to make it mostly configurable. Also, the height of the floor. In the part studio, I tried to design every similar part only once. When I do the pocket hole joinery in the part studio instead of in "2. Assembly “frame half”"I have to insert the same part two or four times. My conclusion is, I can design something (for example a dowel) in an assembly in two parts, but not nothing (for example a hole) in two parts (only if I use context editing).

Many thanks to all for your help and ideas.

1. part studio “wood” (in document named "Holz")

2. Assembly “frame half” (in document named Gestell_halb)

3. Assembly “frame” (in document name Gestell)

4. Assembly “workbench” (in document named Werkbank)

nick_papageorge073

I went through your model and you did a nice job. I had a few questions/comments:

1) Why did you build the 3 (before they were split) platte parts in the studio on top of each other, instead of where they would go on the real workbench? That makes it confusing to visualize the design as you're building it. I'm sure you had a reason:)

2) Why did you split the frame sub-assy into two identical halves? Is that how it will be built in your shop, then join the two halves together? Or was it for a CAD reason?

3) Is the top subassy meant to slide on and off of the frame after the bench is built? Or will it be permanently attached to the frame.

4) You can fix one of the parts in each subasssy to remove the degrees of freedom.

nocry3

I have read some parts probably 5 times, but because of translation difficulties, I don't understand everything exact

1) Why did you build the 3 (before they were split) platte parts in the studio on top of each other, instead of where they would go on the real workbench? That makes it confusing to visualize the design as you're building it. I'm sure you had a reason:)

I always have the problem of knowing when to use a Part Studio and when to use an Assembly. If I model the whole workbench with exact positions in Part Studio, I never need an assembly. Is it better to model everything like in reality directly in the Part Studio? But then I have to create the same parts several times in Part Studio?

2) Why did you split the frame sub-assy into two identical halves? Is that how it will be built in your shop, then join the two halves together? Or was it for a CAD reason?

I am an employee of a university and this model is for a course “Product Design”. The first step is to model the prototype of the workbench on a 3D printer. Bridging is an issue with 3D printing, hence the two halves, which should be printable separately. At present, however, it is not yet possible because of the “blue-gray” medium struts.

3) Is the top subassy meant to slide on and off of the frame after the bench is built? Or will it be permanently attached to the frame.

I do not understand this question. Which sub assembly do you mean? What should slide on and off?

4) You can fix one of the parts in each subasssy to remove the degrees of freedom

A ok. Is it better to fasten one part to the origin or set one part to 'fixed'?

eric_pesty

nocry3 said:

I always have the problem of knowing when to use a Part Studio and when to use an Assembly. If I model the whole workbench with exact positions in Part Studio, I never need an assembly. Is it better to model everything like in reality directly in the Part Studio? But then I have to create the same parts several times in Part Studio?

Here's a good "general" best practice rules for this: if you are creating parts within a single part studio, they should be created in their "proper" location. However you should only create one of each part (and then add multiple instances in an assembly)
If you find yourself just creating separate parts "on top of each other" at the origin, they should probably go in separate part studios.

In this case using a variable studio and/or deriving a reference sketch as needed would help implement that.

It's good practice to "fix" (rather than mate to origin) one part in each assembly, preferably in a "logical" spot relative to the origin (even though assembly origins don't mean a whole lot in Onshape...)

nick_papageorge073

nocry3 said:

I have read some parts probably 5 times, but because of translation difficulties, I don't understand everything exact

1) Why did you build the 3 (before they were split) platte parts in the studio on top of each other, instead of where they would go on the real workbench? That makes it confusing to visualize the design as you're building it. I'm sure you had a reason:)

I always have the problem of knowing when to use a Part Studio and when to use an Assembly. If I model the whole workbench with exact positions in Part Studio, I never need an assembly. Is it better to model everything like in reality directly in the Part Studio? But then I have to create the same parts several times in Part Studio?

2) Why did you split the frame sub-assy into two identical halves? Is that how it will be built in your shop, then join the two halves together? Or was it for a CAD reason?

I am an employee of a university and this model is for a course “Product Design”. The first step is to model the prototype of the workbench on a 3D printer. Bridging is an issue with 3D printing, hence the two halves, which should be printable separately. At present, however, it is not yet possible because of the “blue-gray” medium struts.

3) Is the top subassy meant to slide on and off of the frame after the bench is built? Or will it be permanently attached to the frame.

I do not understand this question. Which sub assembly do you mean? What should slide on and off?

4) You can fix one of the parts in each subasssy to remove the degrees of freedom

A ok. Is it better to fasten one part to the origin or set one part to 'fixed'?

1) Use both, on nearly every design! Use a part studio for a small assembly like this workbench, and draw the parts where they will be in real life. However, only draw one of each part, like you did with the leg. So you would not draw 4 legs in the studio, only one. Then when you go to the assembly, you insert all the parts by selecting the entire studio in the insert dialog. Group all the parts, and fix (or mate to origin) one of the parts. Then, for the parts that are missing, such as the other 3 legs, assemble those individually. This way you get the best of both worlds. Your part studio is intuitive during the design process, but it does not have duplicates of parts. And your assembly BOM (bill of materials) is accurate in that it would have qty 4 of the leg, rather than qty 1 of 4 identical legs if you had mirrored them in the studio.

2) Makes sense.

3) The subassy called Tischplatte. Maybe you made it separate for 3d printing reasons like #2?

4) Fix is easier. However, mating to the origin can be more reliable. I'd probably start with fix unless you end up having issues with parts shifting.

Check out this custom feature called multi-mate-connector. It's helpful in designs like this when mating in the assembly, if you want to use mates rather than group.   https://cad.onshape.com/documents/5d8da63844bedebe5cff72b1/v/a2f8d68037aff39e9d20f7a1/e/629230d0d394845d93416361

nocry3

Thank you for your tips and help. They have helped me a lot. I have completely redesigned the workbench and made it configurable. But it is not finished yet. Now I have two more problems/questions:

1. In the configuration, I use a scaling divisor for simple size changes, e.g., 10 for 1:10. The divisor appears in every configurable dimension in the sketch, e.g., #Tabletop_Length/#Scaling_Divisor (German: #Tischplatten_Laenge/#Skalierungsteiler). Now I have two configurations, "Default" and "3D-Print". How can I include the #Scaling_Divisor as a column? I only manage to do it with the entire expression "#Tabletop_Length/#Scaling_Divisor".

2. The tabletop should have a grid of holes, with a diameter of 20 mm and a distance of 96 mm from hole center to hole center. Depending on the size of the tabletop, there should be different numbers of holes. The distance between the table edge and the center of the first hole should be at least 120 mm, for example. I have created a complex formula that calculates the number of holes and the exact edge distance >120 mm for the length and width of the tabletop, so that a row of holes runs exactly through the middle. But how do I get this configurable into a sketch that also works?

Document-Url