Any general guidelines to maintaining associativity or not?

[kev h]

Hi

Just assembling 1st whole mould tool and seems to be ok if a bit slowly

Just woundering if you guys have any general rules with maintaining associativity when projecting faces to create other parts in place within assembly as just worried i might be tieing myself in knots with out knowing it :roll: . Or is it just 100% a matter of experience??

Also getting an error about unable to open a couple parts but then continues to open them correctly which seems fine but just a little worring?

Cheers Kev 8)

 

[NateLiquidGravity]

I've found that projecting sketches with association between different parts in an assembly is very flaky. Instead I tend project without association move it a little and just dimension or constrain to the edges. For some reason this seems to update better! :wink: :? :roll:

 

[kev h]

Hi Nate

Thanks for reply , with the kinda info i was after.

Inter design constraints is something i'm not too sure about either and why italics suddenly appear and disappear sometimes when all seems to be fine.


The Error I mentioned previously can be seen in the attachment below but as i said seems to load up ok.??

Cheers Kev 8)

 

[dwc]

I use association when projecting to sketches all the time without problems.
I would go crazy if I didn't have this possibility which saves me great amounts of work.

Interdesign constraints are a different story.
I am not sure what causes them (if someone could please explain them?) and they always create problems so they get deleted sight unseen if I find one in the constraint tree.
Hope this helps,
Don

 

[bigseb]

and why italics suddenly appear and disappear sometimes when all seems to be fine.

Maybe I'm mentioning the obvious but an assembly can take a while to fully load, even though it already shows on the screen. I think it all depends on the size of the model and your cpu. My laptops aren't too quick. If I was to load something like my lunch box mould assembly (which is huge, over 550 parts) then it takes a long time to load. Even when it finally shows on the screen the constraints are all in italics; give it another 30 seconds to a minute and its fine again.

To your screenshot: can I just ask where your G: is? If your saving directly to a flash drive there may lie your problem.

 

[DavidJ]

Interdesign constraints are a different story.
I am not sure what causes them (if someone could please explain them?)...

I believe they are created whenever you project to sketch between parts and select 'maintain associativity'. In which case an aspect of the design of one part is linked to something in the other part. If you don't select 'maintain associativity', it is a 'once only' copy and no permament linkage is created.

 

[kev h]

Yep on flash drive as been taking between work and home so kept folder with all items in it on there. Why is that a prob ?

Interdesign constraints are a different story.
I am not sure what causes them (if someone could please explain them?)

Glad it isnt just me

Am i to assume that italics are just a warning that something might not work out or does something definatly need sorting out ?

Thanks for help.

Cheers Kev 8)

 

[BernardK]

The workflow I use is to create reference sketches with 'maintain association' and 'create reference figure' selected. These reference lines can be left untouched unless they need to be deleted. I then create independent entities that form the outline and use co-linear, equals and concentric constraints as appropriate to constrain to the reference lines. This makes it easy to delete the IDC and recreate it without interfering with the outline geometry. I have found this method to be very effective and prevents a number of other side effects.

 

[kev h]

Hi Bernard

Thanks for reply and might give that method a go but doesnt it still associate to the previous part but with an extra link in the chain that shouldnt be deleted?

Cheers Kev 8)

 

[BernardK]

Yes. that is correct.

My experience is that editing an entity with an IDC, such as a trim or extend, will remove the constraint. Secondly, if the entity is part of the outline and it is deleted and re-inserted, the 3D feature takes on a new internal reference number. The effect of this is to upset any constraints associated with the feature, e.g. mates or aligns. Alibre does not tell you that constraints have been deleted and it may be some time before it is apparent.

As an example, I have used IDCs to create mortice and tenon joints. It is quite easy to model the tenon on to one part and then use project to sketch to get the outline for the second part. Once the mortice is created, mates and aligns are used to constrain the two parts together. Now if I need to remodel the mortice and end up deleting the associated sketch and re-drawing it, the mates and aligns may get deleted along the way. If the outline remains in tact, and the reference sketch is deleted it is a simple process to reconstrain a new reference sketch to the existing outline and all remains a nice day.

I might try to look through some examples of this and put a tutorial together. You are right that it introduces additional steps that, in principle, are redundant. My experience is that separating the IDC from the outline makes them much more reliable to implement. It is very frustrating to find that parts that were once constrained are no longer constrained and the reason is not too obvious.

 

[kev h]

Thanks Bernard , great explanation , especially about the editing removing IDCs.

Certainly learning loads with this mould tool , and now customer has just informed me that he needs next size up die set for the tool which will be fun adjusting !! :roll:

Cheers Kev 8)