Reference pattern

[Jholt]

Hi,
I am moving to Alibre from a background in PTC/Creo ( although it has been a long time)
Is there something analogous to the "reference pattern" in Creo?

What I am trying to do is this:
Say I have part "A" which is a flange with a bolt circle. The bolt circle created using a circular pattern.
In an assembly I create a mating part "B" and line it up to "A" with constraints, but it does not have a matching bolt circle.

In Creo I was able to make a single hole in "B" by referencing geometry of the pattern leader in part "A". when I went to pattern the hole in "B", it automatically followed the pattern created in A, creating a matching bolt circle.

Is there a similar feature in Alibre? I like to have my hole patterns driven in as few places as possible so that I don't have to dig around in a bunch of parts to make a change.

Thanks,
Jenn Holt

 

[HaroldL]

Jenn,
Alibre is not that sophisticated, yet. You will have to create the pattern for the bolts independent of the hole pattern. For the pattern axis you can select an edge or face of the flange. You can also edit the pattern to add parts, say nuts and washers. Also, if the hole pattern skips a location you can edit the pattern in the Design Explorer to delete the bolt, nut and washer for the missing hole.

Another, more involved, possibility is to use a Global Parameters file to drive the design.

 

[simonb65]

In an assembly I create a mating part "B" and line it up to "A" with constraints, but it does not have a matching bolt circle.

In the assembly workspace, editing 'Part B here' (which allows you to edit Part B whilst still using Part A as reference geometry), you can use Part A holes in the assembly to project to sketch on Part B and maintain association, so that if you change the pattern on Part A, Part B will follow. Which sounds similar to ...

In Creo I was able to make a single hole in "B" by referencing geometry of the pattern leader in part "A". when I went to pattern the hole in "B", it automatically followed the pattern created in A, creating a matching bolt circle.

 

[Jholt]

Harold,
Thanks for the response. There is always a learning curve with new software learning the new/different features.

I have another pattern question, but I'll start a new thread for it.

Jenn

 

[Jholt]

In the assembly workspace, editing 'Part B here' (which allows you to edit Part B whilst still using Part A as reference geometry), you can use Part A holes in the assembly to project to sketch on Part B and maintain association, so that if you change the pattern on Part A, Part B will follow. Which sounds similar to ...

Simon,
Thanks for your response. I had figured out how to use the "project to sketch" option to bring in geometry to my sketch. Is this what you mean?

My normal use case for this is that the holes in one part are tap drill sized and the others are clear, so I can't use the projected features directly since the holes are different sizes. If there are only a few holes, it is no problem to draw them using the projected references. and the holes update accordingly. It is just tedious to draw a bunch of new features in the sketch if there are a lot of holes. It also fails if you change the number of holes (ie going from a 6-hole pattern to an 8-hole pattern)

I can work around this, it was just a nice feature I had gotten used to in Creo.

Jenn

 

[simonb65]

Thanks for your response. I had figured out how to use the "project to sketch" option to bring in geometry to my sketch. Is this what you mean?

My normal use case for this is that the holes in one part are tap drill sized and the others are clear, so I can't use the projected features directly since the holes are different sizes. If there are only a few holes, it is no problem to draw them using the projected references. and the holes update accordingly. It is just tedious to draw a bunch of new features in the sketch if there are a lot of holes. It also fails if you change the number of holes (ie going from a 6-hole pattern to an 8-hole pattern)

Yes that's what I was meaning and yes. it's a bit limiting if you change the number of holes in the pattern, but is a simple method if your just match tooling a set size pattern or even need to just ensure the hole sizes stay in sync.

 

[simonb65]

You can use the hole feature in the assembly workspace to match drill/tap holes through multiple parts, but you can't pattern feature that in the assembly! So, either way it's a bit of work to get where you need to in Alibre, but it's doable.

 

[bigseb]

Four ways to do this:

Another, more involved, possibility is to use a Global Parameters file to drive the design.

1) GPs are the best way to do a ton of stuff in AD. Place one hole in the part using GPs to define the position and then circular pattern using GPs to determine the instances. Create the opposing part the same way.

2) Catalogue feature. Downsides are that you will have to manually place each hole withing the hole feature tool and you cannot edit this later on. But if the bolt circle is fixed then this will save you a ton of time.

3) Old school. Create the hole and circular pattern for each part individually. Works but tedious.

4) Boolean subtract. Create a separate part that is essentially a pattern of shafts that match the diameter of the bolt holes and patterned accordingly. Then simply boolen subtract that part from your flange to create the bolt circle.

 

[HaroldL]

In Creo I was able to make a single hole in "B" by referencing geometry of the pattern leader in part "A". when I went to pattern the hole in "B", it automatically followed the pattern created in A, creating a matching bolt circle.

That sounds like what SolidWorks has in a couple of options for patterning components in upper level assemblies, Sketch Driven Patterns and Pattern Driven Patterns. Where I used to work I used the Sketch Driven Pattern quite often to install fasteners in the assembly and pattern them to the sketch that controlled the hole pattern in the component part two levels down. To reference the sketch it was just a matter of drilling down in the Feature Manager to the hole pattern sketch on the part, select it as the driving sketch then select the fastener(s) to pattern in the assembly. Any change in the pattern at the part level propagated up the assembly to the top level. All the patterns would update the BOM table as well. That is a feature I'd like to see implemented in Alibre. In a way, the Alibre Hole tool uses a sketch driven pattern now. Once you place the hole or holes you want any changes are made to the sketch controlling the pattern. It would be a real treat if the Hole sketch could be referenced for patterning the fasteners that install into those holes.

In the assembly workspace, editing 'Part B here' (which allows you to edit Part B whilst still using Part A as reference geometry), you can use Part A holes in the assembly to project to sketch on Part B and maintain association, so that if you change the pattern on Part A, Part B will follow.

Simon, I've not had good luck using Project to Sketch in assemblies. While this may work when changing the hole size and bolt circle diameter I don't think this method will update if there is a change in the number of holes. Can you clarify? Thanks.

 

[Max]

1) GPs are the best way to do a ton of stuff in AD. Place one hole in the part using GPs to define the position and then circular pattern using GPs to determine the instances. Create the opposing part the same way.

This.

 

[DavidJ]

You can also add nodes in Hole Tool, or circles of desired size in a standard cut, then constrain these concentric with holes in the first part (whilst editing here).

 

[simonb65]

Simon, I've not had good luck using Project to Sketch in assemblies. While this may work when changing the hole size and bolt circle diameter I don't think this method will update if there is a change in the number of holes. Can you clarify? Thanks.

I find it works very well for some things, but as you say and as mentioned previously, it's not suited to changes in the 'number' of holes, or tracking pattern changes, etc. There just isn't a way to create the additional projections automatically. Good for fixed patterns though when you just need to change holes sizes.

I use project to sketch in the assembly technique a lot, but not for bolt holes, my usage is for PCB edge connector cut outs in enclosure panels. You can project the edges of the connector on the PCB assembly to the panel part, add a clearance and associate the projection, then if I have to move a connector on my PCB, the panel hole follows. Good for some applicatIons, but not patterns!

Solutions given in the last few posts are the way to go.

Inter-design pattern associations would be a really nice cool feature to have though!