LABEL WITH TEXT IPT.

[zorann]

Hi 

I have created an ipt. file of a label with some text on it. It's just a simple rectangle with some text extruded as a cut.

every time i try to modify something on this label it takes agonisingly long.

Am I doing something wrong or am I pushing Inventor to it's absolute limits. 

It's frustrating, it's time wasting. If anyone knows of any solution with this please help.

Every new release of this stupid software brings some innovations, but they never fix simple things that never work in this software.

It hurts my brain to use this software for my work every day.

[Yijiang.Cai]

If you would like to quickly edit the text value, please see the attached part. When changing the value of label, the text will be updated. It will save the time to edit the sketch text.

[jhackney1972]

We don't want your brain to ache too bad!  Maybe you need to learn a little more about Inventor before you go calling it a "stupid" application.  This is a very intensive process since text has so many sketch segments.  You will get a lot better, not instantaneous, results if you use the "Emboss" command instead of extrude.  It was created for this purpose.  Plus you get to choose the color of the text surface.  This selection icon is often missed in the dialog so I am giving your a screen capture to make sure you can find it.  Your file is attached in Inventor 2018 format, which you forgot to mention, modified to use the Emboss command with a top color of Black.

[zorann]

Hi 

I have used Inventor for better part of 15 years. It has same issues that never get addressed with every new release.

I understand what you are saying about the text and that it has many sketch segments in it, why can't Autodesk offer solution to this that works. i used to use "Emboss" until i was told by one of the Autodesk guru's that I was better off using extrude as it was meant to process it more efficiently. Same as being told to use LOD to better handle large assemblies, but in recent times we are told not to use LOD but use View Rep. instead. It is all very confusing.

So many years of Inventor new releases and it still can't handle large patterns in assemblies in a timely manner.

And so on...

[johnsonshiue · Accepted solution]

Hi Zoran,

The part you attached was created in 2009. I used an internal debug tool to migrate all features to 2018 (the last saved version). Now, the edit and update seems to be fast. Could you take a look?

Regarding the difference between Extrude and Emboss, there is indeed some difference. Extrude takes a profile to sweep along the sketch normal direction in a given distance. Emboss, on the other hand, uses the profile to split the given faces and then thicken the split face to the given distance. For planar faces, the resultant geometry from either feature is the same. But, for non-planar faces, they are different. Certainly, Emboss is slightly more compute intensive. However, there should not be drastic difference. There could be bugs in the past leading to one being much faster than the other.

Regarding LOD and Design View Rep, I personally believe there was miscommunication and misunderstanding. LOD was designed to be memory management tool. It was essential to enable users to design assemblies requiring more memory than allowed on 32-bit Windows. However, for some reasons, some users have tried using it for Configuration purposes. For some cases, it does work. But, for most cases, LOD is not an adequate Configuration tool. It cannot alter BOM or PartsList. Changes to multiple LODs cannot be saved at the same time. In drawings, each LOD has to be loaded in the memory if it is referenced by drawing views.

Starting from Inventor 2016, you can specify Design View Rep as a filter to deduct invisible components in Drawing PartsList. So, you can use DVR to control part quantities in the drawing. However, there is still only one BOM table in the assembly as single source of truth.

I can tell that you are unhappy with using Inventor. Inventor is a tool of choice. It has its own strength and weakness. But, we are committed to improve it consistently. If you have any further questions or comments, please feel free to post them here. We have experts around the world answering questions around the clock. You are also more than welcome to contact me directly ([email protected]).

Many thanks!

[zorann]

Hi Shiue

First of all, thank you for taking time to look at this. I am sorry if I let my frustration get better of me.

It is possible that attached part was created in 2009 and saved copy of a few times. However I don't understand why it had to be migrated to 2018 version as our software provider migrates all files in our Vault every time we upgrade to later version of Inventor.

I would like to ask a few more questions at later time (I have a meeting to go to for the rest of my day), concerning use of LOD and DVR if possible? Just wanted to make sure that we are currently using both techniques for correct applications when used in larger assemblies

Regards Zoran

[johnsonshiue]

Hi Zoran,

You are more than welcome. I am not bothered at all. I do understand sometimes it can be frustrating to use a tool if it does not do what you want it to do.

Regarding migration, it is a broad topic. There is file level migration, meaning a given file is migrated to a given release format. Then the earlier Inventor releases can no longer open the files. The "migration" I did was on feature level. When a part or assembly feature is created, it is tagged with a birthday. The birthday stays forever until the feature is deleted and recreated (or updated). The file migration does not alter the birthday. The birthday tells Inventor how the given feature needs to be computed to keep compute stability. We do have an internal tool to "update" the birthday so that the features are computed in the latest and greatest algorithm. I think your part benefits from this process.

Certainly, you are more than welcome to ask any Inventor-related questions here or directly to me ([email protected]).

Many thanks!