Newly installed font not extruding

[rjethwa]

Hi there... I have a logo designed which I need to extrude onto the surface of a part.  I have copied the font into the Creo 11.0.0.0\Common Files\text\fonts folder, and the font shows up in the Font list Sketching > Text dialogue box.  I can write out the logo onto the surface, but it doesn't seem extrude.

I cannot spot any node gaps either.

The font is a really common Windows font: Berlin Sans FB.  Is anyone able to see if you can extrude any words using this font?  Unfortunately, this site doesn't allow me to attach a copy of the font but it should be in your Windows folder if you use.

I'm really puzzled

[StephenW]

somethiing about a specifc letter maybe. 

EDIT: The r doesn't work, all the other letters in your text  aviyo work 

[MartinHanak]

Hi,

• I downloaded berlin-sans-fb.zip from https://font.download/font/berlin-sans-fb
• I unzipped berlin-sans-fb.zip and copied BRLNSR.TTF to E:\PTC\Creo11_020\Creo 11.0.2.0\Common Files\text\fonts directory
• I started Creo 11.0.2.0 and created extrude successfully

Edit: Font I used looks different from your font. Where did you get your font?

[rjethwa]

Thanks @StephenW and @MartinHanak 

So it turns out that I can do that myself but that's only when the text is pretty large.  When I shrink so text has a height of 6mm, I get the following warning:

I have changed the model accuracy to 0.0001 and the extrude works; anything larger than this and the extrude fails.

But what's the downside of lowering the accuracy to this bottom limit? File size? Speed of regen?... other?

The other option I tried was to save the logo as a .dxf file and apply to the sketch as a logo, but this create an insane number of curves (preceded by a program warning). And even on this, a couple of nodes do not join and hence I join manually, but the extrude still doesn't work.

Thanks

[tbraxton]

If you are using start parts that predate Creo 7 then you may have the accuracy of the part set to relative rather than absolute. Prior to changing the accuracy in your model, what was the accuracy setting in the part (relative or absolute)?  If the part is using relative accuracy, then that is likely the cause of the issue.

[rjethwa]

I'm using 11.0 at the moment, but I cannot recall which version I used to create the parts in the first instance.  Is there a way to check?

And I have checked the accuracy of a handful of the other parts and they are all 'Relative' 0.0012

What's the actual impact or complications I can expect?

Of the 20ish parts in total, there are only 2 parts that I have had to change the accuracy on in order for the logo to be extruded.  If there's a better way of adding the the logo, then that would be great.  Is there a way of adding the logo to a sketch so that it doesn't behave as a series of editable curves (i.e. it was a pdf outline) that can be extruded?

[tbraxton]

This relative accuracy is almost certainly the cause of your issues. If you have parts with relative accuracy, then the start parts almost certainly predate Creo 7. In Creo 7 + PTC has only used absolute accuracy. You should immediately update your start parts and use absolute accuracy for all of them. Absolute accuracy should always be used and not relative accuracy.

Relative accuracy is dimensionless and changes with the model bounds, absolute accuracy has units of length and is fixed unless changed by the user.

See this thread for some background info an accuracy settings and how to change them: ACCURACY FROM RELATIVE TO ABSOLUTE CREO 7 - PTC Community

[rjethwa]

Changing to 'Absolute' is easy for me.  I have just tried with one part and it's flipped easily to the following:

Perhaps I did create all these parts in 11.0... 🤔

Before I do the switch for all parts, am I going to have to do any further steps of checking or anything on each part after I have flipped?  Just want to understand what I'm getting myself into.

Thanks so much so far.. 🙂

[tbraxton · Accepted solution]

Specific details matter in this context. In general, if you change the accuracy and the model fully regenerates then you are good in the context of that model. Accuracy is critical in data sharing (copy geom, merge etc.), if you use any of the top-down data sharing features then all models of a design should share the same accuracy setting (absolute with the same value). If use multibody modeling, then all models in a design space also must have the accuracy matched.

I would not just accept the floor value that Creo is offering when you set the accuracy as this value will be different among models and render them incompatible with data sharing functions. Lower accuracy setting will increase regeneration time. In light of this you should set the value low enough to resolve the smallest feature you need on a model. This varies with design requirements and manufacturing tolerances of the processes used to make the parts. If your mfg process can hold +- 0.001" then I would set the model accuracy to be 0.0001" as an example. This ensures that Creo should always reproduce features as small as 0.001" without any issues in the geometry kernel. 

I would really encourage you to work out an acceptable absolute accuracy setting for your use case(s) and set up start parts for that ASAP. You will potentially be in a world of pain if you have a complex design geometry that is failing due to an accuracy mismatch between models. I have had to fix this type of issue for clients in the past and it usually requires that we recreate their design data using proper techniques from start parts, not fast or inexpensive to resolve.

[rjethwa]

Thanks for this detail. I plan to flip each part to Absolute and see note down the accuracy the app defaults to. Then I'll identify the lowest value across the board and change the accuracy to this value across all parts. I guess this will meet the requirements you suggest?

Must admit, none of this seemed to be an issue when I have 3d printed the pieces so far (and I appreciate 3d printing is very low resolution). The on screen accuracy I was working with, practically, was 0.1mm, and all the parts will be high pressure die cast in an alloy. I just wonder in these instances what an accuracy of many many more decimal places will impact. Still, happy to learn 😊.

Thanks

[MartinHanak]

---

@rjethwa wrote:

Thanks for this detail. I plan to flip each part to Absolute and see note down the accuracy the app defaults to. Then I'll identify the lowest value across the board and change the accuracy to this value across all parts. I guess this will meet the requirements you suggest?

Must admit, none of this seemed to be an issue when I have 3d printed the pieces so far (and I appreciate 3d printing is very low resolution). The on screen accuracy I was working with, practically, was 0.1mm, and all the parts will be high pressure die cast in an alloy. I just wonder in these instances what an accuracy of many many more decimal places will impact. Still, happy to learn 😊.

Thanks

---

Hi,

from my point of view it does not make any sense to set absolute accuracy to low value because of extruded text. It is necessary to investigate the font and find out why it is causing problems.

I am repeating my previous question ... Where did you get your font?

[rjethwa]

Hi Martin, OK, thanks for that. 

Honestly, I cannot remember exactly where I got the font from - it would've been one of the free font sites. I've found here >> https://online-fonts.com/fonts/berlin-sans-fb

I've used the font in Inkscape, Word, PowerPoint, etc, and it always shows as I expect per attached screenshot.

If you can suggest an alternative then happy to compare this against @tbraxton.

To be clear, the height of the final text 'raviyo' needs to be 6mm, and reverse extruded to about 1.2mm

Many thanks!

If you can 

[MartinHanak]

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@rjethwa wrote:

Hi Martin, OK, thanks for that. 

Honestly, I cannot remember exactly where I got the font from - it would've been one of the free font sites. I've found here >> https://online-fonts.com/fonts/berlin-sans-fb

I've used the font in Inkscape, Word, PowerPoint, etc, and it always shows as I expect per attached screenshot.

If you can suggest an alternative then happy to compare this against @tbraxton.

To be clear, the height of the final text 'raviyo' needs to be 6mm, and reverse extruded to about 1.2mm

Many thanks!

If you can 

---

Hi,

if you "cannot remember" then pack your ttf file into zip file and upload it. This way I will get font you are using.

[tbraxton]

I agree with @MartinHanak that use of a TTF font should not ordinarily require a change of accuracy. If you would post a version of your model where you attempted to use the font before you made any changes suggested in this thread, it would enable us to review it for potential issues related to the problem (regeneration).

You should confirm the provenance of the font as Martin has suggested as well.

[rjethwa]

Hi guys - I have attached the font as a zip file (BRLNSR.zip). 

And I also attach the part onto which I have added the text using the same font (see Sketch 2 layer):

I have included the failed extrude as well.

The part, without any adjustments, has the following accuracy:

Looking forward to your feedback!

Thanks

[tbraxton]

As I had suspected based on the error message for your regeneration error when you attempted to use 6 mm text height you have a part using relative accuracy. If you use absolute accuracy (of a magnitude to avoid the tiny edge) this error is not present. The extrusion of the text is creating a tiny edge that when using the default relative accuracy causes the regen failure.

As I explained previously do not ever use relative accuracy unless you have an explicit reason to do so, it only invites problems. PTC uses absolute accuracy by default since Creo7.

I am not discounting an issue with the font file but the regen error is due to an edge that is too small to resolve when using relative accuracy at the default value.

[MartinHanak]

---

@rjethwa wrote:

Hi guys - I have attached the font as a zip file (BRLNSR.zip). 

And I also attach the part onto which I have added the text using the same font (see Sketch 2 layer):

I have included the failed extrude as well.

The part, without any adjustments, has the following accuracy:

Looking forward to your feedback!

Thanks

---

Hi,

I investigated the shape of letter "r" and realized that its shape is problematic. Please replay attached font_problematic_locations.mp4 video.

• 1st location shows bug in shape definition
• 2nd and 3rd  locations show short elements

Note: Your model is saved in educational version therefore I cannot open it.

I agree with tbraxton and his suggestion to set absolute accuracy.

I do not have any other suggestions ...

[rjethwa]

Hi Martin - yes, it seems like some nodes don't meet properly even when I use the font directly in the application. Previously, as I mentioned, I created the text in a graphics app (Inkscape) and imported as a .dxf; even when I did this, there were some rogue nodes which I couldn't fix.

Thanks for all your help. All much more clearer now