Frame Generator - creating holes from skeletal model sketch

[mjc_design]

Hi all

In Inventor 2016, is there away I can use sketch hole crs from the skeletal model to create top level holes in my frame? Lines from the skeletal model sketch are obviously used to create the frame members, but why can I not use hole crs to create holes in the frame?

Thanks

Matt

[mdavis22569]

Can you share an example?

Are you not able to project geometry? 

Turn on the sketch first  ...

[mjc_design]

hopefully you see the hole crs in my skeletal model sketch over the frame, but I can't use those hole crs to create holes in the frame

[mjc_design]

to answer your other question, if I create a sketch and project the hole crs they're not linked to the original so won't update. 

[mdavis22569]

You can make them adaptive no?

[mjc_design]

Nope, when I project them they have a padlock on them. Sketch cannot be made adaptive either.

Also, I completely forgot i'm using Inventor 2017 not 16

[mdavis22569]

Can you share it .... via a pack and go?

[mjc_design]

sure, here we are...

[mdavis22569]

While I can do the holes ... I can't get them adaptive .... looking for other options ....

[johnsonshiue]

Hi! There are two logical reasons to the behavior you are describing. 1) The sketch is an assembly sketch. Adaptive sketch does not apply to assembly sketch. 2) The target sketch exists in a part which is already adaptive in another assembly context. A part can only be adaptive within an assembly, not multiple assemblies.

Many thanks!

[mjc_design]

@johnsonshiueThe sketch exists within the part, that is being used for the frame generator. Sketch geometry can be used for frame members, but not for holes in the frame it appears. This is quite a shame to be honest.

I understand that frame generator copies the geometry into its own skeletal model, but it would be really useful if there was some similar functionality to use sketch geometry for other features. As frame modifications have to be done at the top level, having the sketch unadaptive is no help either...

[kelly.young · Accepted solution]

Hello @mjc_design was looking at this, you might have to redesign the whole thing in order for it to work, not sure but might be worth a try:

• On the assembly top level sketch create a dimension from the outside edges to the Origin Center Point.
  • This will stay the same across all parts so you have a shared point for measurement.
  • The reason why this could work is if you Project Geometry or Dimension from the edge it makes a Fixed Constraint in the top level assembly sketch instead which is where the issue you are having.
  • The origin is fixed and the dimension can be driven by a known linked User Parameter.
• Inside the PALLET MASTER part, once the origin reference point is used for location, check Export Parameter from the Parameters.
• When creating a sketch at the top level assembly you can then Link the dimensions as User Parameters. 
• These should update along with the model. 

That probably doesn't make much sense, here is a screencast to clarify:

Hope that helps!

Please select the Accept as Solution button if a post solves your issue or answers your question.

[mjc_design]

@kelly.youngThank you for taking the time to look at this. Your solution certainly works, and I will consider exporting user parameters in the future. I think this might be a bit too long winded for me to do this for every hole though. 

Something I've used is creating work axis' on the points of the sketch, then using the axis to position a cylindrical item in the assembly. I can then project geometry from these items to my assembly sketch, and still have it linked.

Matt

[rayessle]

Ok. So this method adds a couple of steps to creating the holes but you can get them to update from the part through to the assembly.

2manDat

The basic steps are as follows.

1. For every hole centre in your part add a point work feature.

2. In the assembly add an axis work feature using the point from the part and a surface at right angles to the direction you want the hole to be for every hole you need.

3. create a sketch in the assembly on the surface you need the holes.

4. project the axis work features to give you sketch points.

5. Use this sketch to create your holes.

As the sketch in the assembly is projecting work features also in the assembly, the points are associative. The axis work features are also associative to the point work features in the part so everything updates when you change the part.

Screen cast and inventor files attached.

Ray Esslemont

57441584-ab25-4ab4-b1fc-14f3a5cdc56f

Inventor 2018

[rayessle · Accepted solution]

Can't seem to get the screencast to show so trying again.

Regards

Ray Esslemont

[mjc_design]

Thanks, i'd considered doing something similar and it looks like it works well. I haven't tried but could you use point work feature instead of an axis in the assembly? No that there's a huge difference, but work points look neater and for a single hole a point is sufficient.

Matt

[rayessle]

Yes you can use the work point. I only prefer using the axis because when you are doing a lot of holes you can lose track of which ones you have already done. if you put a point on top of a point you can't tell which one is in the part and which one is in the assembly. having the axis stick up helps me to keep track of which ones I have done.

Regards

Ray Esslemont

Inventor 2018