Add Part from Productivity in Assembly - Incorrect units and unexpected zoom out

[steve_lindley]

I've got two issues here in Inventor Pro 2018.1; one I need help with and the other is just a whinge!

In an .iam I'm creating several adaptive new parts. So I click on Add Part, from the Productivity section of the Assembly ribbon. I can browse to a folder, name it, wait for it to appear in my browser pane and start designing no problem.

However, the problem I have is that the part files are defaulting to using cm instead of mm, despite all our part templates having mm. The assembly has mm so it's not that either. I can't find any setting in the options that defines which template to use when using this work flow. Am I missing something? I've seen a thread on this forum from a few years back with a similar issue when creating simplified parts, so I suspect this is a bug, but the solution for that doesn't help here.

Secondly, (this is my whinge) after clicking to edit a new part, I choose Start 2D sketch but before I can click on the plane or face I want to sketch on, the assembly zooms out. It's not going to the home position (which we normally set to as Fit to View) because if I click on the home icon it shifts slightly. It is highly annoying though, because in a complex assembly and in the transparent state for editing in place, it makes finding the surface I want to sketch on very difficult. It's clearly not an issue with looking at a sketch plane on creation, as I haven't yet defined the plane. I can of course create a work plane first, (which is what happens automatically when I create a sketch first anyway) and I shall have to adapt my work flow to do this, but in the interest of reducing the number of clicks it would be better if we didn't have this zoom. Anyone else found this?

Kind regards

Steve

[salariua]

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@steve_lindley wrote:

I've got two issues here in Inventor Pro 2018.1

However, the problem I have is that the part files are defaulting to using cm instead of mm, 

Secondly, (this is my whinge) after clicking to edit a new part, I choose Start 2D sketch but before I can click on the plane or face I want to sketch on, the assembly zooms out. ...Anyone else found this? 

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For the first part, this is the article on simplified part units so you might want to give that a tr.

For the second part (whinge) you can press F5 and it will revert to previous view... I do that EVERY SINGLE TIME my view gets skewed by invoking the sketch command.

[steve_lindley]

Thanks for your reply Adrian.

I've seen that articale and the workaround was "In the Create Simplified Part dialog box, click the icon for the Browse Templates tool." However, in my work flow, I don't have a dialogue box with an option, only a box to give my new part a name and location.

Secondly, many thanks for the F5 suggestion. I didn't know about that keyboard shortcut, so I'll definitly be trying that.

[salariua]

well... leverage our strengths while @johnsonshiue or @ChrisMitchell01 will investigate this.

Here's a workaround for you. Open your assembly and use the Create Component rather than Add Part on Productivity Pack.

Copy paste that file several times in the assembly, essentially creating multiple occurrences of the same blank part but which should have correct units.

Select first occurrence in the browser or graphical window and use the Save Replace button on the Assemble tab Productivity section. Give the file a name.

Select second occurrence (copy) and do the same....

you should only make sure you have enough blank copies in the assembly but you can always create one with New Component.

I use Save Replace so often that I even gave it a shortcut key "SR"

[johnsonshiue]

Hi Steve,

Let me embed my reply to your post so it would be easier to read. Please let me know if more information is needed.

Many thanks!

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@steve_lindley wrote:

I've got two issues here in Inventor Pro 2018.1; one I need help with and the other is just a whinge!

In an .iam I'm creating several adaptive new parts. So I click on Add Part, from the Productivity section of the Assembly ribbon. I can browse to a folder, name it, wait for it to appear in my browser pane and start designing no problem.

However, the problem I have is that the part files are defaulting to using cm instead of mm, despite all our part templates having mm. The assembly has mm so it's not that either. I can't find any setting in the options that defines which template to use when using this work flow. Am I missing something? I've seen a thread on this forum from a few years back with a similar issue when creating simplified parts, so I suspect this is a bug, but the solution for that doesn't help here.

[JS]: I am not able to reproduce the behavior. Add Part command simply insert a new part based on Standard.ipt. Could you check and see what unit Standard.ipt has? Do you have Standard.ipt? If not, you can easy get it (Tools -> Application Options -> File -> Configure Default Templates).

Secondly, (this is my whinge) after clicking to edit a new part, I choose Start 2D sketch but before I can click on the plane or face I want to sketch on, the assembly zooms out. It's not going to the home position (which we normally set to as Fit to View) because if I click on the home icon it shifts slightly. It is highly annoying though, because in a complex assembly and in the transparent state for editing in place, it makes finding the surface I want to sketch on very difficult. It's clearly not an issue with looking at a sketch plane on creation, as I haven't yet defined the plane. I can of course create a work plane first, (which is what happens automatically when I create a sketch first anyway) and I shall have to adapt my work flow to do this, but in the interest of reducing the number of clicks it would be better if we didn't have this zoom. Anyone else found this?

[JS]: This is about a controversial behavior in Part 2D Sketch. When you try to create a new 2D sketch and there isn't anything to pick from (no visible body geometry or sketches or planes), Inventor would make origin planes visible temporary and set to Home view. This behavior was meant to help new users that a plane has to be selected in order to create a sketch. When nothing is visible, this requirement is not apparent. There isn't an option to control the behavior. However, there is away to suppress the behavior. Simply in the part template file, make one or more origin planes visible. Next time when you insert a new part, the rotating behavior will be gone.

Kind regards

Steve

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[ChrisMitchell01]

You beat me to it Johnson 🙂

Yes, Add Part simply copies Standard.ipt from the top level Templates folder.

-Chris

[steve_lindley]

Thanks for taking the time to reply (everyone).

@johnsonshiue and @ChrisMitchell01 - We don't use any of the standard templates and when we install Inventor, we point the application options to a network folder, ignoring the templates stored locally, so we don't see the standard.ipt when creating new. However, I took a copy of the standard.ipt and .iam and pasted into our network folder to be able to create new and check their settings. Both are set to mm, which is really what I expected, because as part of our migrating process, we always click on the 'Configure Default Template' button and choose mm and ISO before pointing the software to our templates folder. So I'm still confused as to why the parts default to cm. Also, are we alone in using a network folder for templates? If not, have Autodesk ever considered giving the user the ability to choose the template .ipt when using the Add Part function? Perhaps as part of the application options?

Regarding the zoom behaviour, again thanks for suggestions to prevent this. We don't use the Add Part function very often, so I finished creating the parts I needed by creating new work planes first. My personal preference is not to have origin planes showing, so it wouldn't make sense for me to have them visible for the few times each year this happens, so I'll happily leave it there.

Kind regards

Steve

[johnsonshiue]

Hi Steve,

If I understood the issue correctly, the behavior is caused by the fact that there is no Standard.ipt in the default template folder path. As a result, Inventor does not know which default template you use and it sets to cm. Could you check the following setting and if it is set correctly?

Go to Get Started tab -> Project -> Folder Options -> Templates. What is it set to?

Go to Tools -> Application Options -> Files -> Templates. What is it the default template path?

Even if you don't use any of the Standard templates, it is better to keep them there. Some Inventor workflows do assume the availability of the template files and grab them to create new files. If the default template files are not in the unit you like, you can go to Tools -> Application Options -> Files -> Configure Default Templates. Inventor will change the current Standard templates or create new Standard templates stored in the default template path. Add Part command is more like a semi-automated shortcut allowing users to create a new part in an assembly quickly. If it allows users to select a template, it would function exactly the same as Create command.

Many thanks!

[steve_lindley]

@johnsonshiue

Both locations are set to the same path, for our network folder. So still a bit of a mystery on the cm. It's the same on our other machines so not specific to me either.

We don't really want to keep the standard.ipt in the same folder as we want everyone to use just the templates we've developed. If we rename one of our templates to 'Standard' there's a risk of confusion in the future (if ever there's a change in personnel for example - when installing and migrating), so we don't really want to do that either. I'd be interested to hear how other users manage their templates.

I understand that the Create tool allows the selection of the template and I think I'll personally adopt that work process instead. However, perhaps I didn't explain my suggestion very well. Rather than select a template ever time, in Application Options, alongside the default templates field, if you could select the specific .ipt or .iam files to use for any semi-automated tools, I think this would be more helpful - to us anyway. Select it once and then use the Add Part tool as intended.

Kind regards

Steve

[johnsonshiue]

Hi Steve,

I think I understand the situation. Basically, you simply do not want to use any of Standard templates and you don't want to rename any existing templates to Standard.xxx either. The problem here is that some of the workflows do require the presence of Standard.xxx (Add Part or Import). When Standard.xxx is not available, Inventor will fall back to internal default template, which is the internal unit, cm based.

We have heard similar requirements but the issue here is that the change required to make it work like you wanted is quite significant. So far we have not yet found enough justification to proceed with the change. Please feel free to submit a new idea on Inventor Ideas if there isn't an existing one.

Many thanks!

[SBix26]

We've had our templates in a network folder for many years, but we've always had one of each type named Standard, which in our case is in inches.  We also have Metric templates and a couple of part templates with a basic cylinder and a basic cube already defined.  But the Standard templates mean that automatic processes at least use a template with our preferences, even if the units aren't correct (but are easily corrected).

Sam B

Inventor Professional 2018.1.1
Vault Workgroup 2018.0
Windows 7 Enterprise 64-bit, SP1

[Carl_mgfx]

@johnsonshiue I am having a similar issue to this with my Inventor 2019.3.  I experienced this before and after formatting my laptop.  After my format I installed Inventor 2019 and then 2019.3, the only thing I have done is change the default templates to "millimeter" and "ISO".

My laptop has a clean Windows 10 install (latest version) and the only thing I installed was Inventor and the 2019.3 update.

Now when I use "Add Part" in an assembly with mm units, the new part is inserted with Inch units.

I also have a customer with the same problem.

[johnsonshiue]

Hi Carl,

I need a bit more information about the behavior you are seeing. Let me ask you a few questions and see how we can resolve the issue.

1) Go to Get Started -> Project -> Folder Options -> Templates. What is it set to?

2) You said you change the template unit from English to Metric mm/ISO. How did you do it? Did you go to Tools -> Application Options -> File -> Configure Default Templates?

3) Please take a snapshot of the dialog when you insert a new part and share it here. It will show the exact path the template was used.

Many thanks!

[gilchristj9KHC5]

I had the same issue and changing the name to standard allowed me to add parts in inches rather than cm using the productivity tab.

[AIR_123]

I have the same issue with "Add part" units.
Thanks Johnson for reply. I don't see why implementation is an issue?
Why does IV has to rely on the template for units?
Just add an option in application settings to push certain standard/units system to newly created files.
Then the story with "always carry Standard.ipt to dedicated templates location" is over, right?