Working from parant part in frame generator

[michielXWZ7U]

Hi

In my work i am developing a lot of products that are combinations of steel tubes and laser cutted sheet metal. Most of the time the lasercutted parts need to be adjusted to the size of the inserted tubes. So that they can fit exactly within the frame.

My workflow now is;

- create the skeleton sketch and lasercutted parts all in one parent part

- 'make component' of all the needed bodies to convert them to an assembly

- in the assembly, add the frames through frame generator.

now my problem:

When i adjust the size of the frame members, the rest of part is not trasforming along with the new size of the tubes.

Anyone has an idea how i can use the inserted frame size as a parameter within my parant part?

[michielXWZ7U]

Hi

In my work i am developing a lot of products that are combinations of steel tubes and laser cutted sheet metal. Most of the time the lasercutted parts need to be adjusted to the size of the inserted tubes. So that they can fit exactly within the frame.

My workflow now is;

- create the skeleton sketch and lasercutted parts all in one parent part

- 'make component' of all the needed bodies to convert them to an assembly

- in the assembly, add the frames through frame generator.

now my problem:

When i adjust the size of the frame members, the rest of part is not trasforming along with the new size of the tubes.

Anyone has an idea how i can use the inserted frame size as a parameter within my parant part?

[cadman777]

Hi Michiel,

Can you post a screen capture of what you are doing?

Also, are the laser parts normal user custom made parts or framegenerator parts or iParts or what?

Thanx...

[cadman777]

Hi Michiel,

Can you post a screen capture of what you are doing?

Also, are the laser parts normal user custom made parts or framegenerator parts or iParts or what?

Thanx...

[Gabriel_Watson]

Probably using some iLogic to fetch the frame size parameters (OD, width, etc.) from the first frame member (or average of all), then saving that to the frame assembly in a parameter, then exporting that to be used by your parent assembly.

[Gabriel_Watson]

Probably using some iLogic to fetch the frame size parameters (OD, width, etc.) from the first frame member (or average of all), then saving that to the frame assembly in a parameter, then exporting that to be used by your parent assembly.

[michielXWZ7U]

HI, is there maybe a project you know of that has done something similar. I am not very experienced yet with Ilogic 🙂

[michielXWZ7U]

HI, is there maybe a project you know of that has done something similar. I am not very experienced yet with Ilogic 🙂

[michielXWZ7U]

I attached a .pdf file to make clear what the 3 steps are that i am using

[michielXWZ7U]

I attached a .pdf file to make clear what the 3 steps are that i am using

[Gabriel_Watson]

I see some ways here of retrieving parameters from your subcomponents. If you are using the same type of frame in frame generator, it makes it easier to set which parameter to get from the subcomponent:
https://forums.autodesk.com/t5/inventor-ilogic-api-vba-forum/assembly-parameters-in-subparts-with-il...
https://adndevblog.typepad.com/manufacturing/2013/07/recursively-accessing-parameters-from-an-invent...
https://forums.autodesk.com/t5/inventor-ilogic-api-vba-forum/using-ilogic-to-reference-a-parameter-i...

So, you may have to post in the iLogic forum for this, as it involves some work and other people may have the code already developed for similar matters. The way I see it, you have to:
0- have your plate/sheet metal dimensioned parametrically, according to one custom/user parameter;
1- retrieve the frame size parameter that you need (width, for ex.) from the frame subcomponents);
2- save to your plate the new value for the size.

You can make a rule that you run manually, since I do not think you need this completely automated.

[Gabriel_Watson]

I see some ways here of retrieving parameters from your subcomponents. If you are using the same type of frame in frame generator, it makes it easier to set which parameter to get from the subcomponent:
https://forums.autodesk.com/t5/inventor-ilogic-api-vba-forum/assembly-parameters-in-subparts-with-il...
https://adndevblog.typepad.com/manufacturing/2013/07/recursively-accessing-parameters-from-an-invent...
https://forums.autodesk.com/t5/inventor-ilogic-api-vba-forum/using-ilogic-to-reference-a-parameter-i...

So, you may have to post in the iLogic forum for this, as it involves some work and other people may have the code already developed for similar matters. The way I see it, you have to:
0- have your plate/sheet metal dimensioned parametrically, according to one custom/user parameter;
1- retrieve the frame size parameter that you need (width, for ex.) from the frame subcomponents);
2- save to your plate the new value for the size.

You can make a rule that you run manually, since I do not think you need this completely automated.

[jtylerbc]

---

@Gabriel_Watson wrote:

Probably using some iLogic to fetch the frame size parameters (OD, width, etc.) from the first frame member (or average of all), then saving that to the frame assembly in a parameter, then exporting that to be used by your parent assembly.

---

I think that's slightly overcomplicating it.  Rather than iLogic, you should just be able to link parameters to get the member dimensions into the "parent" part.

Of course, either of these methods is only practical if you are using the Application Option "Overwrite current file for size change."  If you are not, then the file name will change when the member size changes, and either the iLogic or Linked Parameter method will still be referencing the old file name.

[jtylerbc]

---

@Gabriel_Watson wrote:

Probably using some iLogic to fetch the frame size parameters (OD, width, etc.) from the first frame member (or average of all), then saving that to the frame assembly in a parameter, then exporting that to be used by your parent assembly.

---

I think that's slightly overcomplicating it.  Rather than iLogic, you should just be able to link parameters to get the member dimensions into the "parent" part.

Of course, either of these methods is only practical if you are using the Application Option "Overwrite current file for size change."  If you are not, then the file name will change when the member size changes, and either the iLogic or Linked Parameter method will still be referencing the old file name.

[cadman777]

Michiel,

Thanx for the pdf illustration.

Your project has a simple solution, but not the same work-flow as you are using. Based on what I know of how Inventor works, your work-flow is sort of backwards or incompatible due to deficiencies in Inventor functionality.

So, the way I control all parts in a 'mixed' assembly is using 'skeletal modeling'.

That means:

1. you make a main sketch that is only a sketch and has no solids inside it

2. you Derive that main sketch into each individual plate part as the basis of the part

3. you Insert that main sketch into an assembly and make a frame using FrameGenerator on the sketch lines

4. you change the size of your assembly by changing the relevant dimensions in your main sketch and then updating the assembly.

5. find attached an example of 'skeletal modeling'. Open the '_Wireframe...' sketch and change the dimensions or Parameters and see what happens. The only thing is, you can't change the FG member sizes using parameters. You have to do it manually, or else maybe use iLogic to drive them another way.

Notice that I simplified your sketch by deleting the offset sketch. But if you don't want to change the sketch or your work-flow, then you can try using an Excel spreadsheet to drive the sketch and FG length parameter. But I know of no way to change the FG parts using out-of-the-box Inventor, or to get the FG component sizes using out-of-the-box Inventor. You'll have to use iLogic for that, like @Gabriel_Watson says.

[cadman777]

Michiel,

Thanx for the pdf illustration.

Your project has a simple solution, but not the same work-flow as you are using. Based on what I know of how Inventor works, your work-flow is sort of backwards or incompatible due to deficiencies in Inventor functionality.

So, the way I control all parts in a 'mixed' assembly is using 'skeletal modeling'.

That means:

1. you make a main sketch that is only a sketch and has no solids inside it

2. you Derive that main sketch into each individual plate part as the basis of the part

3. you Insert that main sketch into an assembly and make a frame using FrameGenerator on the sketch lines

4. you change the size of your assembly by changing the relevant dimensions in your main sketch and then updating the assembly.

5. find attached an example of 'skeletal modeling'. Open the '_Wireframe...' sketch and change the dimensions or Parameters and see what happens. The only thing is, you can't change the FG member sizes using parameters. You have to do it manually, or else maybe use iLogic to drive them another way.

Notice that I simplified your sketch by deleting the offset sketch. But if you don't want to change the sketch or your work-flow, then you can try using an Excel spreadsheet to drive the sketch and FG length parameter. But I know of no way to change the FG parts using out-of-the-box Inventor, or to get the FG component sizes using out-of-the-box Inventor. You'll have to use iLogic for that, like @Gabriel_Watson says.

[SharkDesign]

Can you do the frame first and then the ladder cut parts?

This way you can project the frame into your multi body part and it'll (should) always update. 

[SharkDesign]

Can you do the frame first and then the ladder cut parts?

This way you can project the frame into your multi body part and it'll (should) always update. 

[jtylerbc]

---

@cadman777 wrote:

5. find attached an example of 'skeletal modeling'. Open the '_Wireframe...' sketch and change the dimensions or Parameters and see what happens. The only thing is, you can't change the FG member sizes using parameters. You have to do it manually, or else maybe use iLogic to drive them another way.

---

This is true - you can't change the FG members using parameters in the layout part (I'm avoiding the use of the word "skeleton" since it has a specific meaning in FG assemblies).  But there is a way around this.

You can link size parameters from the members back to the layout part.  These can then be referenced by sketch dimensions or work plane offset values.  So what actually happens is:

1. You change a member size the normal way using FG methods.
2. The linked member size parameters update in the layout part.
3. Sketch dimensions, work planes, etc. update accordingly and therefore move the plate geometry to match the new frame member sizes.

So even though you still aren't actually controlling the frame member sizes from parameters in the layout part, it adjusts the plates as though you were.  No iLogic or spreadsheets are required for this method - only some time spent linking parameters and setting up your plate sketches to use them in whatever way is necessary to achieve the desired result.

[jtylerbc]

---

@cadman777 wrote:

5. find attached an example of 'skeletal modeling'. Open the '_Wireframe...' sketch and change the dimensions or Parameters and see what happens. The only thing is, you can't change the FG member sizes using parameters. You have to do it manually, or else maybe use iLogic to drive them another way.

---

This is true - you can't change the FG members using parameters in the layout part (I'm avoiding the use of the word "skeleton" since it has a specific meaning in FG assemblies).  But there is a way around this.

You can link size parameters from the members back to the layout part.  These can then be referenced by sketch dimensions or work plane offset values.  So what actually happens is:

1. You change a member size the normal way using FG methods.
2. The linked member size parameters update in the layout part.
3. Sketch dimensions, work planes, etc. update accordingly and therefore move the plate geometry to match the new frame member sizes.

So even though you still aren't actually controlling the frame member sizes from parameters in the layout part, it adjusts the plates as though you were.  No iLogic or spreadsheets are required for this method - only some time spent linking parameters and setting up your plate sketches to use them in whatever way is necessary to achieve the desired result.

[cadman777]

Thanx John for the great idea. The only downside to that is the number of derived Parameters in the master-sketch if the variations in members in your FG assembly are many, or if you use the parameters on a part-per-part basis. Could get very confusing with the G_T_1_2_3_4_5_6....._n, if you know what I mean. Been there, done that!

Another method I use is to save a CC file as a "_Template-...." locally, and then derive the Parameters from that part. Then if the part size changes, you can do what you do. That way, one part covers all the frame members of that size in your FG assembly. That's how I've done it over the years. But still, there are caveats with doing it that way if things change down-stream.

[cadman777]

Thanx John for the great idea. The only downside to that is the number of derived Parameters in the master-sketch if the variations in members in your FG assembly are many, or if you use the parameters on a part-per-part basis. Could get very confusing with the G_T_1_2_3_4_5_6....._n, if you know what I mean. Been there, done that!

Another method I use is to save a CC file as a "_Template-...." locally, and then derive the Parameters from that part. Then if the part size changes, you can do what you do. That way, one part covers all the frame members of that size in your FG assembly. That's how I've done it over the years. But still, there are caveats with doing it that way if things change down-stream.

[jtylerbc]

Since I only derive frame member parameters I'm actually going to use, I find that it's rarely a practical problem for me.  But there is definitely the potential for it to get out of hand if what you're working on is complex enough.

[jtylerbc]

Since I only derive frame member parameters I'm actually going to use, I find that it's rarely a practical problem for me.  But there is definitely the potential for it to get out of hand if what you're working on is complex enough.

[cadman777]

It's like everthing we do w/CAD software.

You have to use the least complicated work-flow, or it bites you in the rear at the end.

[cadman777]

It's like everthing we do w/CAD software.

You have to use the least complicated work-flow, or it bites you in the rear at the end.