Patterns with a Part in a Part (Hole Wizard)?

[JMOS4]

Hi,

I have a Weldment that we added 4 holes with the hole wizard into, this particular place puts weldments (part file) into another part for the machining version or Part into part:

As you can see.

Now in assembly level I try to fix or even add a pattern of fasteners to a hole that is in the base part/weldment, and I get the following error:

So what am I doing wrong or need to do or do I have to now dissolve the previous pattern and mate each fastener one by one?

Regards,
Jim

[JMOS4]

Hi again,

Found this option int the machine part but still does not let me select the hole in a assembly to drive a pattern:

Regards,
Jim

[AlexLachance]

I've never used parts in parts in that manner, but one thing I have learned from parts in part is that selecting from the model window is not the best for features. There's gotta be some kind of feature that you can select from the featuremanager so that you can use the hole pattern to drive a pattern.

[JMOS4]

Hi,

This is all that is in the tree from the original part(weldment)

as you can see no holes to grab in the tree items.

Regards,
Jim

[AlexLachance]

Hi,

This is all that is in the tree from the original part(weldment)

image.png

as you can see no holes to grab in the tree items.

Regards,
Jim

Just a thought, perhaps you could bring the sketches in from the part and do a sketch driven pattern using the sketch that was used for the pattern of the holes. That would give the desired result I believe.

[Frederick_Law]

If you want to edit the weldment, open the weldment.
You can't edit the weldment in assembly or in the part it's inserted to.
If you want to pattern a hole, add the hole in current file.
You can't pull feature up from a child.

[Glenn Schroeder]

I've had good luck with selecting holes in the graphics area to drive Pattern Driven Component Patterns, but I suspect that inserting Part in Part breaks that link when the driving pattern is in the inserted Part.

You said "this particular place." Is this workflow the preferred standard where you work, or are you working with a client's files?

[Glenn Schroeder]

If you want to edit the weldment, open the weldment.
You can't edit the weldment in assembly or in the part it's inserted to.
If you want to pattern a hole, add the hole in current file.
You can't pull feature up from a child.

Frederick,

Maybe I misunderstood, but I don't believe the OP is trying to edit the weldment, but is trying to use a hole pattern to drive a Pattern Driven Component Pattern in an Assembly. The fact that it's a weldment is irrelevant.

[JMOS4]

Just a thought, perhaps you could bring the sketches in from the part and do a sketch driven pattern using the sketch that was used for the pattern of the holes. That would give the desired result I believe.

Hi again,

I can and going to end up converting entities of the edges of the holes and create a sketch to do a sketch driven pattern but makes no sense onto why the functionality of a pattern driven pattern is not available when you do a part in part file.

Hopefully someone has the magic answer or SW adds it, as this should be relatively easy process.

Regards,
Jim

[Glenn Schroeder]

Hi again,

I can and going to end up converting entities of the edges of the holes and create a sketch to do a sketch driven pattern but makes no sense onto why the functionality of a pattern driven pattern is not available when you do a part in part file.

Hopefully someone has the magic answer or SW adds it, as this should be relatively easy process.

Regards,
Jim

While I don't disagree with you, I would also like to point out that using the Part in Part functionality should be used very sparingly, and in many cases using an Assembly would be a better option (and you wouldn't be having this issue if this was an Assembly instead of Part in Part).

[Frederick_Law]

Have fun with your partlist.

[JMOS4]

While I don't disagree with you, I would also like to point out that using the Part in Part functionality should be used very sparingly, and in many cases using an Assembly would be a better option (and you wouldn't be having this issue if this was an Assembly instead of Part in Part).

Hi,

I agree completely, new company and have me doing revisions to existing product.

I have only used the part in part ding castings and even then, not totally sure the logic on how a part in a part is any better or a real reason to go that route vs. part in assembly and add your cuts/holes/machining in the assembly level as this is how most of my past employers have done it.

Regards,
Jim

[TTevolve]

I think the problem is when you insert a part into another part it comes in as a solid body, just like if you open a STEP or IGS, the history is gone for that part in the other part. I think your only choice would be to do a new assembly pattern or not to use the part in the part and use a real assembly.

[SPerman]

You have the option to import more than just the solid body. But it definitely isn't the full history tree.

image.png (12.42 KiB) Viewed 1957 times

[Glenn Schroeder]

Hi,

I agree completely, new company and have me doing revisions to existing product.

I have only used the part in part ding castings and even then, not totally sure the logic on how a part in a part is any better or a real reason to go that route vs. part in assembly and add your cuts/holes/machining in the assembly level as this is how most of my past employers have done it.

Regards,
Jim

I hope they're letting you move away from that for current and future products?

[DennisD]

I use part-in-part for machining castings. It works perfectly for this since at that point the machining is effectively working on a dumb solid. All the machined features have their own parametric definition. Having visibility of the parametric features of the casting is not only clutter, but a recipe for disaster as it makes it too easy to change something. This really cemented itself for us when we learned how to access the casting from the machined part file. Prior to that we just used a single part file with configurations: As Cast, and Machined, but it was far too easy to change a dimension or a feature on the machining and inadvertently push that change into the As Cast configuration. Using part-in-part solved this for us very nicely.

As with anything, there are different ways to achieve the desired results. Opinions will differ, but that doesn't make them wrong. I use assemblies and will mate-drill holes or weld things together just as would be done in making the assembly. But part-in-part is the preferred method for us when doing something like machining a casting, or even modifying a purchased part (such as drilling a hole in a stock fastener, which is making a new part from a purchased part). And frankly, the part-in-part method is a more accurate representation of the steps taken to produce the finished version; it is not an assembly, but a modification of something else after it has been manufactured to that prior level. Using the drilled fastener as an example of part-in-part, the drawing would identify the purchased part and only show the dimensions for drilling the hole. Any dimensions of the fastener itself are by definition reference dimensions.

Now flip that coin over. If we had a single part file of a part with an As Cast configuration and a Machined configuration just imagine the work required for their respective drawings. The As Cast would have all of its feature dimensions show up in the drawing, but they would also show up in the Machined configuration. Doing this as a part-in-part a) makes these separate part files, but still connected, b) makes the drawing easily executed since the Machined part does not show any cast dimensions, except what a person would add for reference.

[JMOS4]

I use part-in-part for machining castings. It works perfectly for this since at that point the machining is effectively working on a dumb solid. All the machined features have their own parametric definition. Having visibility of the parametric features of the casting is not only clutter, but a recipe for disaster as it makes it too easy to change something. This really cemented itself for us when we learned how to access the casting from the machined part file. Prior to that we just used a single part file with configurations: As Cast, and Machined, but it was far too easy to change a dimension or a feature on the machining and inadvertently push that change into the As Cast configuration. Using part-in-part solved this for us very nicely.

As with anything, there are different ways to achieve the desired results. Opinions will differ, but that doesn't make them wrong. I use assemblies and will mate-drill holes or weld things together just as would be done in making the assembly. But part-in-part is the preferred method for us when doing something like machining a casting, or even modifying a purchased part (such as drilling a hole in a stock fastener, which is making a new part from a purchased part). And frankly, the part-in-part method is a more accurate representation of the steps taken to produce the finished version; it is not an assembly, but a modification of something else after it has been manufactured to that prior level. Using the drilled fastener as an example of part-in-part, the drawing would identify the purchased part and only show the dimensions for drilling the hole. Any dimensions of the fastener itself are by definition reference dimensions.

Now flip that coin over. If we had a single part file of a part with an As Cast configuration and a Machined configuration just imagine the work required for their respective drawings. The As Cast would have all of its feature dimensions show up in the drawing, but they would also show up in the Machined configuration. Doing this as a part-in-part a) makes these separate part files, but still connected, b) makes the drawing easily executed since the Machined part does not show any cast dimensions, except what a person would add for reference.

Hi,

I agree there is a place for part in part, but you could effectively do the same with a part/casting or weldment and an assembly file with all the machining done there as for drawings you can have a drawing with a assembly file and all the dimensioning done there, I think people get hung up on the word "assembly" when it is really being used as a operation so to speak OP10, OP20, etc...

I worked at a place that did a part in assembly and had the same part number for both, the part file was the casting or weldment, the assembly was treated as the upper level, as for drawings they contained 1 sheet or set of views of the part file and another set of the assembly file.

Either way not sure why the functionality of a hole wizard item would not transfer in part to part or to allow for a pattern driven pattern in a higher-level assembly.

Regards,
Jim

[JSculley]

Hi,

This is all that is in the tree from the original part(weldment)

image.png

as you can see no holes to grab in the tree items.

Regards,
Jim

There is something wrong with that model, unless I'm missing something in your description of what's happening. Here's what I did:

1. Create a multibody weldment part model. It's a tube with a plate on the end:

2. Create a new part and insert the weldment part and then create some hole wizard features and pattern them:

3. Create an assembly and mate some hardware to the hole wizard features.

4. Try to create a pattern-driven pattern of the hardware using the patterns created in the part from step 2.

5. No problem:

[SPerman]

There is something wrong with that model, unless I'm missing something in your description of what's happening. Here's what I did:

1. Create a multibody weldment part model. It's a tube with a plate on the end:
image.png

2. Create a new part and insert the weldment part and then create some hole wizard features and pattern them:
image.png

3. Create an assembly and mate some hardware to the hole wizard features.
image.png

4. Try to create a pattern-driven pattern of the hardware using the patterns created in the part from step 2.
image.png

5. No problem:
image.png

When you insert the part in the part, do you have "hole wizard data" checked?

image.png (16.27 KiB) Viewed 1874 times

[SPerman]

I see what is going on now. The OP had the hole pattern in "part 1" before inserting it into "part 2." This does not work, even with the "Hole Wizard Data" checked.

The reason Jim's method works, is because he is creating the hole wizard in "part 2", after "part 1" has been inserted.

[JSculley]

When you insert the part in the part, do you have "hole wizard data" checked?

The pattern succeeded, regardless of whether that option was checked or not.

[AlexLachance]

The pattern succeeded, regardless of whether that option was checked or not.

Jim, he is speaking in a part, not an assembly.

He has a part with a hole wizard pattern made in it that was inserted into another part. He wants to use the hole pattern of the inserted part to drive a new pattern but cannot use it because the pattern does not exist inside the part(even with the inserted part having hole wizard data checked).

[JSculley]

From the original post:

Now in assembly level I try to fix or even add a pattern of fasteners to a hole that is in the base part/weldment, and I get the following error:

For what's its worth, I was able to get the error message if I created a hole pattern in the original weldment (say a tap drill for a 1/4-20 hole) and then created a hole pattern in the part-in-part (say a 1/4-20 tapped hole) right on top of the original holes and then tried to pattern fasteners in the assembly by trying to select the cylindrical face of the hole in the model. The fix for this scenario was to select the tapped hole pattern from the flyout feature tree.