Project to sketch.

[DIXON]

Hi All,
Is it possible to use "project to sketch " in an assembly ? ie, I have a part B in said assembly and holes have to be exactly matching the holes in part A in location. I tried to project the holes from A to B but no success [ so far ]

Thanks.

 

[bigseb]

No. I think it won't pick up the other parts' edges if you edit a part 'in assembly'. You can create feature in a assembly, however these don't carry over to the part.

 

[DIXON]

Thanks biqseb, that is what I was finding [ no picking up of edges ] bit of a pain but I will get around it somehow. Would be a very useful feature to have though.

 

[DIXON]

Update, I found that I can achieve what I need, I need to edit the part in the assembly, activate sketch on the face / plane required then I can project the sketch from the inactive part. I must have missed something earlier It works fine if there is a small space between the parts but not sure if it will work if the parts are "mated " Will go and try that soon.

 

[DIXON]

Surely missed out something earlier as it now works perfectly even when the faces are fully mated.

Cheers.

 

[Lew_Merrick]

Dixon -- What you can do is to place reference geometry in your (Edit Here) Part that is "tied" to your Assembled Counterpart and then use those (Reference Points assumed) to locate your mating Holes.

 

[DavidJ]

Project to sketch should work fine if you 'edit here' in assembly mode. Be aware that you are creating an inter-design constraint, which can limit some other options in Alibre. I've used this functionality successfully for many years.

 

[JST]

Project to sketch should work fine if you 'edit here' in assembly mode. Be aware that you are creating an inter-design constraint, which can limit some other options in Alibre. I've used this functionality successfully for many years.

You do NOT have to create an interdesign relation with project to sketch. In fact it is best to avoid that.

The way to avoid that is to create a plane in the target part file for the sketch to project TO. That is key. (and of course do NOT check the box at bottom that asks if you WANT to "maintain association with source".

If you tie the plane to ANYTHING ELSE in the assembly, you will have trouble with interdesign relations. You HAVE TO have a destination plane IN THE TARGET PART FILE.

The simple case is if the plane is actually a surface of the part. Then you can use that as the plane, or create a separate plane (better) that does not depend on the part surface (which might change).

If you do that, then the outline that you project will go into the part as if it were an undimensioned sketch (it's good to dimension it), which has NO relation back to the assembly, it is just a "snapshot". You will need to manually update it if mating parts change, but that is maybe better than the alternative, because you will know when to do it, what to do, and how to do it.

IF you instead tie to some surface or plane in the assembly OTHER than the affected part, it will still work, but you WILL have an "interdesign relation", and it will almost certainly end up biting you in the backside when you are not expecting that.

The problem is that if that other part, plane or surface moves, the interdesign relation will cause it to move in the affected part which it was projected to, as well. Odds are that will end up breaking some constraint(s), and your design explorer will light up as red as a mass murder scene. if that happens, you may be "S.O.L." because it will be really hard to untangle.

 

[jfleming]

I have avoided using inter-design relations entirely. It's caused too much headache, rework, and frustration to even bother with it.

 

[DIXON]

Thanks to all for the help with this. I have sussed it out now. I have noticed some problems with inter design relations so now can do it as JST suggested and all is fine.

Cheers.

 

[Lew_Merrick]

I have avoided using inter-design relations entirely. It's caused too much headache, rework, and frustration to even bother with it.

Actually, the only "problems" I have had with Inter-Design Relationships can all be traced to improperly laid-out or configured Parts or Assemblies.

 

[JST]

I have found that while they look like a great idea, and they really DO work OK........ kinda....

They also seem slow down the computer horribly, and sometimes seem to refresh all the data from ground zero every time the viewpoint is panned. That leads to display delays, overshoots on panning, and general issues, if more than one or possibly two are active.

If it were not for that, I'd consider using them, because the actual idea behind them is really super. If not for the confusion problem of all sorts of inter-relations, they would be an ideal tool in some cases.

I think I'd want to be able to set them up, have them active in the design stage, and then be able to "cut the link" without a problem, when the parts are all stable.

Unfortunately, that does not seem to work well. When I have deleted an interdesign relation, the last configuration has not been preserved reliably, it seems to sometimes have reverted back at least one change level, and maybe more. I do not think it was a matter of saving, I don't know just what went wrong.

 

[jfleming]

Actually, the only "problems" I have had with Inter-Design Relationships can all be traced to improperly laid-out or configured Parts or Assemblies.

That's fine, I started using Inter-Design Relationships when I first began using Alibre. I know now that I was doing it incorrectly then and that resulted in the issues that I had. Too many fish in the frying pan now to learn the right way to utilize it.