Sheet metal cut through multiple bodies

[foolishgrunt]

I use multi-body sheet metal parts to design individual housing panels (using derived parts), and I have a two part problem.

1) When I want to cut a single rivet hole through two separate bodies, I can only use the sheet metal cut feature if the bodies are the same thickness. Is this a feature or a bug? It seems like a bug. My workaround has been to use the extrude cut feature rather than the sheet metal cut when I'm going through multiple bodies, but that leads me to my second issue.

2) When I create a drawing of the individual derived parts, only the holes that were created by the sheet metal cut feature can be called out using the hole tag. For holes that were created using extrude cut, the hole tag does not recognize the feature and does not attach - for these I have to use the standard dimension tool. Is this a feature or a bug? I understand that it may be a feature, but it significantly impacts the workaround for my previous issue.

[mikejones · Accepted solution]

Hi

You're correct that the SM cut feature won't create the cut through two bodies of different thickness in one go. You can however do it in two steps by sharing the one sketch but this is a two step process. If you're putting holes in for rivets why aren't you using the hole function instead as that will put the hole through multiple bodies of varying thickness in one go.

Mike

[johnsonshiue · Accepted solution]

Hi! I am sorry I am not sure I understand the issue. The cut can go any depth. As long as the depth penetrating multiple bodies, it does not matter what thickness it is.

The second issue sounds  like a bug to me. Please check the Doc Settings in the drawing. Go to Tools -> Doc Settings -> Drawing -> Default Automatic Centerlines -> make sure all feature types are selected.

If possible, please share an example that exhibits the behavior here.

Many thanks!

[mikejones]

Hi Johnson

The issue with the cut command now is that although you can specify to cut through all it isn't possible to select more than one solid at a time. You can deselect the current solid and choose a different one to cut but it is impossible to select more than one solid. I suspect this is a bug.

I remember within the last two weeks that someone else was having problems using the hole callout on extruded holes but I'm not sure what the outcome of that one was.

Mike

[IgorMir]

Hi Johnson;

Here is a model (IV2020) which explains the issue. Cut1 goes only through the plates of 6mm. thick.  It doesn't go through the 3mm. thick plate. The same applies to the Cut2. It only goes through 3mm. thick plate. Yet on both occasions the Cut is set to All. BTW - it makes no difference even if it is set to "To" and picking the opposite face of the whole set of plates, or specify the distance of, say 50mm. It still cuts through the plates of the same thickness only. There is no option to add a plate with a different thickness to the Cut set.

Hole1, on another hand - can be drilled through by picking all the solids individually. But even if the hole termination is set to Through All - it still goes through by picking one solid at a time.

Another question is - why the thickness of the material can only be set twice? I want Face3 be 10mm. Thk., Face2 - 6mm and the Face1 - 3mm. But if I alter the thickness for Solid3 - it affects Face2 as well.  Face1 stays as 3mm. still.

Cheers,

Igor.

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@johnsonshiue wrote:

Hi! I am sorry I am not sure I understand the issue. The cut can go any depth. As long as the depth penetrating multiple bodies, it does not matter what thickness it is.

The second issue sounds  like a bug to me. Please check the Doc Settings in the drawing. Go to Tools -> Doc Settings -> Drawing -> Default Automatic Centerlines -> make sure all feature types are selected.

If possible, please share an example that exhibits the behavior here.

Many thanks!

---

[melrosecad]

Tested this in 2021. It seems you just can't select bodies made from a different material thickness. Using a normal extrude cut works as usual though.

I am not seeing the same situation with your last point. I can set more than two thicknesses of material.

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@IgorMir wrote:

Hi Johnson;

Here is a model (IV2020) which explains the issue. Cut1 goes only through the plates of 6mm. thick.  It doesn't go through the 3mm. thick plate. The same applies to the Cut2. It only goes through 3mm. thick plate. Yet on both occasions the Cut is set to All. BTW - it makes no difference even if it is set to "To" and picking the opposite face of the whole set of plates, or specify the distance of, say 50mm. It still cuts through the plates of the same thickness only. There is no option to add a plate with a different thickness to the Cut set.

Hole1, on another hand - can be drilled through by picking all the solids individually. But even if the hole termination is set to Through All - it still goes through by picking one solid at a time.

Another question is - why the thickness of the material can only be set twice? I want Face3 be 10mm. Thk., Face2 - 6mm and the Face1 - 3mm. But if I alter the thickness for Solid3 - it affects Face2 as well.  Face1 stays as 3mm. still.

Cheers,

Igor.

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@johnsonshiue wrote:

Hi! I am sorry I am not sure I understand the issue. The cut can go any depth. As long as the depth penetrating multiple bodies, it does not matter what thickness it is.

The second issue sounds  like a bug to me. Please check the Doc Settings in the drawing. Go to Tools -> Doc Settings -> Drawing -> Default Automatic Centerlines -> make sure all feature types are selected.

If possible, please share an example that exhibits the behavior here.

Many thanks!

---

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[IgorMir]

Thanks, Ben! 🙂

[johnsonshiue]

Hi Ben and Igor,

I think I understand the issue. This is about the ability to cut sheet metal bodies with different thickness values. It seems like a limitation to me. Technically, it should be doable just like Extrude Cut. However, Cut is more than that. It can do Cut Normal and Cut Across Bend (both are for single body only), heavily depending on body thickness. So, it is limited to multiple solid body in the same thickness value.

Regarding Thickness, you will need to use Sheet Metal Rule to drive the body thickness. Right-click on each body -> Set Sheet Metal Rule. The Thickness should be set to the rule thickness value. If not, it will be a bug. Please share an example.

Many thanks!

[melrosecad]

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@johnsonshiue wrote:

Hi Ben and Igor,

I think I understand the issue. This is about the ability to cut sheet metal bodies with different thickness values. It seems like a limitation to me. Technically, it should be doable just like Extrude Cut. However, Cut is more than that. It can do Cut Normal and Cut Across Bend (both are for single body only), heavily depending on body thickness. So, it is limited to multiple solid body in the same thickness value.

Regarding Thickness, you will need to use Sheet Metal Rule to drive the body thickness. Right-click on each body -> Set Sheet Metal Rule. The Thickness should be set to the rule thickness value. If not, it will be a bug. Please share an example.

Many thanks!

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This was my understanding on this as well. Due to features that rely on the sheet-metal rules.

Your second point works as expected for me in 2021.

Cheers.

[IgorMir]

Hi Johnson;

Thanks for looking into it, much appreciated.

I did share an example. And I have explained (I hope - clear enough 🙂 ) what is happening with the setting of different thicknesses in the file. It might be a bug in IV2020. Ben has mentioned that IV2021 is free from that deficiency.

Cheers;

Igor.

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@johnsonshiue wrote:

Hi Ben and Igor,

Regarding Thickness, you will need to use Sheet Metal Rule to drive the body thickness. Right-click on each body -> Set Sheet Metal Rule. The Thickness should be set to the rule thickness value. If not, it will be a bug. Please share an example.

Many thanks!

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[johnsonshiue]

Hi Igor,

I am sorry I cannot seem to reproduce the behavior on 2020 either. Please take a look at the attached part. Each body can be assigned to a different Sheet Metal Rule with a different thickness value.

Many thanks!

[IgorMir]

Hi Johnson;

Yes, in your file the part works as it is supposed to.

Cheers,

Igor

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@johnsonshiue wrote:

Hi Igor,

I am sorry I cannot seem to reproduce the behavior on 2020 either. Please take a look at the attached part. Each body can be assigned to a different Sheet Metal Rule with a different thickness value.

Many thanks!

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[foolishgrunt]

Gentlemen,

My apologies for being late to return to this thread, and my thanks for continuing the discussion in my absence.

@johnsonshiueYour suggestion worked: selecting the "Cylinder Features" option in the "Automated Centerlines" dialog made it so that the hole note attaches to the extrude-cut hole, so thank you for that advice. Thank you also for the likely explanation of why the SM cut only applies to bodies of the same thickness.

@mikejonesTo answer your question about why I don't use the hole feature, the simple reason is that I forgot it was an option. 🙂 This part has other punched shapes that are not simple circles, and since the hole feature isn't an option for those, I guess I inadvertently forswore that feature for the entire part. But I tested it now and confirmed that it cuts both bodies as desired, and also confirmed that the hole call note attaches to it in the drawings (even with only "Hole Features" selected in the "Automated Centerlines" dialog), so that too is a perfectly reasonable workaround.