2019 HOLE COMMAND - SKETCHED

[avaya2012]

I am using Inventor 2019 Pro.  We have been using 2019 for a month or so now.  First of all, I am not a fan of the updated hole command at all.  It doesn't look terrible but it's a pain every time I change a diameter or length.  You have to click in just right place.  On to my issues/questions...

I use a lot of copied and pasted sketches to put holes in parts.  I cannot start my hole command and then highlight all of the circles to create the holes.  I have to go through and click each one, which brings up another issue.  If I miss my center point I have a hole where ever I clicked which can cause all kinds of issues.  It doesn't appear I can drag and drop to my sketch.  Is there a way to do this?

I also saved a couple of my common hole sizes in the very top box thinking this would be very handy.  This works fine until I try to change a hole size.  I have 9/16" and 11/16" saved.  Lets say I make a hole 9/16 but I realized it needs to be 11/16.  If I edit my hole, click in the very top drop down box and change it to 11/16 nothing actually happens.  This could also cause issues.  Why doesn't it change?

Thanks,

Cody

[mcgyvr]

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@avaya2012 wrote:

I am using Inventor 2019 Pro.  We have been using 2019 for a month or so now.  First of all, I am not a fan of the updated hole command at all.  It doesn't look terrible but it's a pain every time I change a diameter or length.  You have to click in just right place.  On to my issues/questions...

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I have also complained about this to the developers and I'm hoping they address that in a future (soon) update..

I will post a link to this thread in my discussion thread with them on the beta site to show that there are other users concerned about it too..

As to your other 2 issues..

Much of that is just how you are used to working the "old way".. The process has changed some and some adaptation is required..

can you include a sample of your copy/paste problem so others can clearly see what you are referring to? Even a screencast would be helpful..

same for the hole size defaults.. I'm not sure I'm following you exact steps and a specific workflow is required for it to work properly.. Most of that is just learning that new workflow..

[avaya2012]

I figured I may just be working the "old way" on some of this.  You can actually ignore the part about the memorized hole sizes and the very last bit in the screencast.  I set up the name of my common holes but didn't actually change the diameter. 

Not being able to highlight the sketch is still a nuisance.  But I can highlight before I open the hole command, if I remember.  And the "floater" holes if I miss-click.

I hope the screencast loaded fine.  

[johnsonshiue]

Hi Cody,

The highlighted statement is not true. You can always add points or center points to Hole command. These circular centers are not picked up automatically because they are not the so-called sketch center points. You can either use window-select to pick these points to add to an existing hole, or change their type to sketch center point so they will be picked up automatically. This workflow has not been changed. It works like this before 2019.

Many thanks!

@avaya2012 wrote:

I am using Inventor 2019 Pro.  We have been using 2019 for a month or so now.  First of all, I am not a fan of the updated hole command at all.  It doesn't look terrible but it's a pain every time I change a diameter or length.  You have to click in just right place.  On to my issues/questions...

I use a lot of copied and pasted sketches to put holes in parts.  I cannot start my hole command and then highlight all of the circles to create the holes.  I have to go through and click each one, which brings up another issue.  If I miss my center point I have a hole where ever I clicked which can cause all kinds of issues.  It doesn't appear I can drag and drop to my sketch.  Is there a way to do this?

I also saved a couple of my common hole sizes in the very top box thinking this would be very handy.  This works fine until I try to change a hole size.  I have 9/16" and 11/16" saved.  Lets say I make a hole 9/16 but I realized it needs to be 11/16.  If I edit my hole, click in the very top drop down box and change it to 11/16 nothing actually happens.  This could also cause issues.  Why doesn't it change?

Thanks,

Cody

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[avaya2012]

Did you watch the screencast I posted?  The highlighted statement is 100% true.  I cannot "window select" the circular centers while the hole command is active.  I have to select each  circular center individually, which can lead to errors if the center is missed.

[johnsonshiue]

Hi Cody,

I was not aware that you were talking about creating holes at assembly level. It should work like in a part. It looks like a bug to me. I will work with the project team to understand the behavior better.

Many thanks!

[mcgyvr]

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@johnsonshiue wrote:

Hi Cody,

I was not aware that you were talking about creating holes at assembly level. It should work like in a part. It looks like a bug to me. I will work with the project team to understand the behavior better.

Many thanks!

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@johnsonshiue Window select of sketched or projected circles and their circle center point doesn't work in a part either..  

[johnsonshiue]

Hi Cody and Brian,

Another episode of human multi-threading error stroke me. I am sorry I was confused. Indeed, the issue here is that regular sketch point (non-center point) cannot be window-selected. I believe this might be a change in design to avoid picking up unneeded points. The workflow right now is that you will have to change the point type to Center Point so that they can be selected automatically.

I still need to double-check with project team to confirm the behavioral change and see what we can do.

Many thanks!

[Jelly_Liu · Accepted solution]

Hi Cody,

We will add an option to let user choose whether select center-points only or not when window-select. Just as Johnson said, current design is to avoid misselecting unneeded points, which is non-center sketch points.
There is a User Story (INVGEN-16116) in our backlog. We will let you know when this function is done.

Thanks for your feedback!

[mcgyvr]

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@Jelly_Liu wrote:

Hi Cody,

We will add an option to let user choose whether select center-points only or not when window-select. Just as Johnson said, current design is to avoid misselecting unneeded points, which is non-center sketch points.
There is a User Story (INVGEN-16116) in our backlog. We will let you know when this function is done.

Thanks for your feedback!

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@Jelly_Liu Jelly, Is there a user story to increase the padding/spacing in the fields?

Its too close and as a user I'm often accidentally clicking the arrow to the right opening that dialog or placing my cursor before the last letter causing an incomputable value.. 

Specifically I'm talking about this area..

There needs to be more open spacing there to not require such precision in mouse placement to go in and select/highlight/change the value..

This should apply to all fields in this new dialog.. 

[kmiller]

For us we used the From Sketch option on the part levels daily by numerous people.  So this new hole command will actually be a performance hit for us.  I did test doing window selection so at least you can still do that, but to have the From Sketch placement option would still be nice so you don't have to try to windows select everything.  We may have one sketch span out across a whole building because it's on a particular "level" and I can see where window selection would slow us down.  Just my 2 cents. 

Added - looks like from sketch is still an option on the assembly level, but not on a part level. - third time edit is a charm... maybe.. 

[Davarn-ToolGuy]

Disappointed, is an understatement over what I feel about the 2019 "improved hole command."

Without the ability to project holes from multiple blocks onto a base plate and then window select those holes we are going to revert back to an earlier version. 

Being able to select a random spot on a sketch without any geometry also is problematic. I have heard complaints of near misses to the actual desired spot resulting in holes being inaccurate.

Unbelievable. 

Lastly, Why was this thread marked "Solved"?  It's not solved until it is solved.
Dave Arnold

[johnsonshiue]

Hi Dave,

Based on our internal record, the ability to window-select sketch points will be included in the coming 2019.2 update. You will need to install 2019.2 update on top of 2019 RTM build.

Many thanks!

[Davarn-ToolGuy]

I updated the software, figured out the correct setting and now it allows window selection of the projected holes.  Consider this solved. 

Thank you Johnson Shiue.

[johnsonshiue · Accepted solution]

Hi Dave,

Many thanks for your confirmation! I am sorry that it was not available immediately when we shipped Inventor 2019. It was an omission. We did make the change in 2019.2 based on the feedback we got.

Thanks again!

[avaya2012]

I got it figured out.  The correct settings are kind of hidden. 

For anyone else that is looking, you need to open the hole command, click the three lines in the upper right corner of the dialog box, then un-check "window select center points only." 

[Anonymous]

With the old hole function you could also switch to points in a different sketch. You can't do this anymore and for me this is a really important missing feature. Sometimes it happens that you need to move holes to a different sketch (lets say from a shared one). You could just unselect them and re-select on another sketch, but not anymore. Hope this will get fixed too.

[johnsonshiue]

Hi Dejan,

If I understood your request correctly, it is still doable on 2019. You either unselect the point in the graphic window or clear the selection in the dialog. Have you installed 2019.3 update?

Many thanks!

[Anonymous]

Not if the point you want to select is on another sketch. I have 2019.3 and when you de-select all points you can only choose the points on the same sketch as the original points. You used to be able to switch to another sketch completely with the old tool.

If I remeber correctly with the old tool you just had to switch to the type of hole definition(linear or cocentric hole or whatever), reselect and then click OK. Then re-edit the feature to sketch hole with points on another sketch selected. It would be nice if you could extract the information from a hole feature and re-use it.

[johnsonshiue]

Hi Dejan,

I think I understand it now. This is about the ability to change consumed sketch from one to another on edit. Unfortunately, the workflow is indeed removed. It is because the hole feature from 2019 is essentially a sketch-based feature (a sketch is needed) instead of mixed-types (sketch or workpoint or edges optional).

I don't believe you can switch from a sketch hole to a non-sketch hole and then back to a sketch hole. This workflow no longer exists since it is always a sketch-based feature. The current behavior is consistent with Extrude or Revolve, not allowing to select a different sketch on edit. We are aware of the deficiency and we are trying to improve in future releases.

Many thanks!