Extrusion Length not in FX list

[serpennica]

Inventor 2023.

Issue is, No FX extrusion length. Where did it go.

When i do an extrusion I am selecting between feature then I use two working plans as my "TO" and "FROM" work plane distance. they are the angled work planes.

The dimension is shown in extrusion pop up with parentheses (86.703). when I hover over dimension it say d2 is my function.

The problem is, I do not get this dimension (d2) in the FX list. I want to export this distance to my bom list.  

P.S, frame generator is not the go to solution, there are more problems there.

file attached, could not figure out how the pack n go correctly.

[ampster40]

can confirm the parameter does not exist but noticed also there is no where you can pull that dim from, that would be my guess as to why there is no parameter?

[serpennica]

the best I can do is go back to original sketch and put a reference dimension.  that shows up in FX.

I was wanting to get full length of part, but that seams not so. the model will have about 40 parts like this, just was looking for an easy way to show full length of pipe. the extrusion is just center length, but that won't work because of angle end cuts.

[blandb]

Why not use frame generator as it will display the correct length needed?

[serpennica]

frame generator does not give me  the flexibility with the part. Frame generator gives to many folders to work with. It does not allow me to move the part. yes I can move a sketch line, but it does not allow me to re-associate the part with a different sketch line. any changes to a part would be a recreation of a new part and a new file. frame generator does not allow me to keep the same part and relocate it. I wish I could have the frame generator trim/extend etc.... features in  the part file, would make a top down assembly build much better. I have parts with custom iProperties and I loose that information every time i change frame generator parts. Frame generator is best for set it an forget it, but there is always a change or revision and frame generator does not support single parts to retain customization.

the simple task of getting length of part can't  be accomplished, without many steps. It should not be that hard. the information is already there.

[blandb]

You can customize folder structure in your Application Options > File Tab > File naming defaults.

You can re-use components as well (as long as the line lengths are the same length). So, if you do add holes to one item and need that else where, you do not have to recreate the part. 

You can move parts once they are placed, You can choose the "Change" command to move a member off the sketch line in the A/B and rotation options vs altering the sketch line location. This is similar to the "move bodies" command in the single part file you are dealing with.

I'd like to see how "complex" your frames are and why this is "too complicated" for frame generator? 

Sounds to me you are using the default installed libraries vs. copying and creating your own company specific library where you can add all these custom iproperties and they are there when placed with FG.

The same file you sent, there are multiple parts (solids) in a single part file. Is this your typical workflow, then do "make components" to get the individual members? Or, do you plan on having a master sketch and then deriving out the master sketch and then making the members that way? Just curious.

[serpennica]

from the pic you have. yes I can see that the frame member can change. The question is. How do I locate that piece to another sketch line. When the change frame feature is used, thats all you get is change frame not relocate. What i want to do is "select line". how to make that frame piece go to another line. When you originally start to place a frame under "insert frame" you get Placement "select line". that is the only time you can locate the pipe piece. I can't relocate the pipe. there's more issues but that is the just one. Any suggestions, 

I work on crane builds, I have to make lattice boom and crane frames. Lots of diagonal and crossing beams.

I attached a build, just the same as before, but started the Frame Gen Assembly.

thank you for you time.

[serpennica]

this would be and example of the diagonal crossing bracing. this could be pipe or tubing.

[blandb]

You can only "reuse" members for lines that are the same length. So, that that case, only your top and bottom members are the same length, so you should be able to reuse a member for it. The other diagonal members gradually get smaller or larger depending on how you look at it and are not the same, so therefore you would not be able to reuse them since they are truly different length parts.

I have attached a sample frame (2024) It is made of a bunch of reused components. I have also moved some off of the sketch lines just to show that you can still manipulate as needed. Hope it helps.

[blandb]

Here is a sample of a job similar to what you show, but we didn't get it. Unfortunately I can't show the whole thing.

[pcrawley]

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@serpennica wrote:

...The question is. How do I locate that piece to another sketch line.

You can't relocate an FG component onto another sketch line after it has been placed.  I know it's useful very occasionally, but generally it's no more than 2 clicks to delete and re-place.  I do understand there are a tiny set of circumstances where it would be useful to relocate a FG member - like after you've done a ton of manual edits to the part and don't want to re-do them.  To work round that scenario, I edit the original sketch, select the sketch entity, delete all the sketch constraints on it (there's an option on the right click menu) - then just moved the entity and constrain it in the new place.  When you exit the skeleton part, the edited frame member follows the original line to its new location.  

[kacper.suchomski]

Hi

This Extrusion has no length - because you haven't defined it.

This is the distance range from - to. But from the perspective of logic, it is not a length, but a range.

You haven't defined length, so you don't have a length parameter.

The value controlled in brackets in the Extrude operation window is a readout, not a parameter.

This means that you need to change your design strategy and adapt it to the expected effects (not only geometric, but also in terms of data and information).

[serpennica]

thanks for the comment, but what you say is only half truth. yes I have not specified the length parameter, but the program calculated the length as a reference distance, yours is d3 (40). that d3 is not given in FX. So my question is. Why did they hide the dimension and not list it as a reference dimension in FX. I understand what you are saying, but Inventor showed the parameter and used it. However, this is only center to center distance, if there is an angle cut on ends the length would have to compensate for the additional angle. 

Using work planes to extrude to and from works better because surface geometry changes and work planes don't. I use work planes and move them as the design develops. 

thank you for your time

[kacper.suchomski]

You didn't understand what I wrote.

D3 position is not a parameter for me.

Parameters are used to define geometry.

Measurements are used to read values.

D3 would be a parameter if it defined a distance.

But it doesn't define; this is read only (just like a dimension in a 2D drawing - this is not parameter).

[k.hendrickx]

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@kacper.suchomski wrote:

Parameters are used to define geometry.

Measurements are used to read values.

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By that logic, why do we have the "reference" parameters at all than?

These "parameters" are also not defining geometry, but are defined by it, yet they are available in the Fx window.

I understand the question from the OP, it would be helpful to have that value available under the reference parameters for future use in other formulas, BOM's, drawings and so one. 

It's up to the user to keep in mind that these values can differ A LOT from the actual length of profile you need due to how it's cut.