topic Re: Inventor Drawing Dimension Lines Partially Disappearing in Inventor Forum

Inventor Drawing Dimension Lines Partially Disappearing

Anonymous — Fri, 19 Jan 2018 23:07:08 GMT

Hi all,

Something I came across and have not figured out why is that my dimensions are partially disappearing in one location. I am sure it has something to do with the template however I have dug through it only to find nothing wrong. Anyone have any ideas? Here is a screen shot. (Beneath the 6.367 & above the 30 deg) It is as if there is a hidden text field (rectangle shaped) that is in this area but can not find it.

kelly.young has edited your subject line for clarity: Dimensions disappearing

Re: Inventor Drawing Dimension Lines Partially Disappearing

cbenner — Fri, 19 Jan 2018 23:07:42 GMT

Can you post the drawing and related part files here? (use pack n go) Very hard to tell without digging in.

Re: Inventor Drawing Dimension Lines Partially Disappearing

Anonymous — Fri, 19 Jan 2018 23:08:01 GMT

Check the 6.367 dimension and make sure you don't have any blanks in the text. Also window select the area and see if there is something there you can't see.

Re: Inventor Drawing Dimension Lines Partially Disappearing

Anonymous — Fri, 19 Jan 2018 23:13:06 GMT

I attempted the select window and nothing showed. There are no additional information in the text field. I redone the drawing to show that it happens anytime. Let me know your thoughts. Thanks in advanced.

Re: Inventor Drawing Dimension Lines Partially Disappearing

JDMather — Fri, 19 Jan 2018 23:13:21 GMT

Still no files, I I'll assume there is some reason you cannot attach the files here and end all doubt.

Double click on the 6.376 (or whatever it was) dimension and post screen shot here.

Re: Inventor Drawing Dimension Lines Partially Disappearing

Anonymous — Fri, 19 Jan 2018 23:13:36 GMT

recheck for files

Re: Inventor Drawing Dimension Lines Partially Disappearing

cbenner — Fri, 19 Jan 2018 23:13:50 GMT

Unsure yet as to why, but there is indeed a "dead zone" in that spot. If you drag the view down a bit it's all good. Delete everything down to bare bones (formats, t-blocks, symbols etc), and place a fresh view... the dead spot is tehre. Same part model placed into one of my templates has no dead spot. So the dead spot is somewhere in your template file, but I haven't found it yet.

EDIT:

It only seems to affect dimension lines and leaders. Are these new templates? Have you ever seen this before? Anything else new about this template file?

Re: Inventor Drawing Dimension Lines Partially Disappearing

Anonymous — Fri, 19 Jan 2018 23:14:06 GMT

Add a new sheet, move the views to the new sheet and delete sheet 1.

Re: Inventor Drawing Dimension Lines Partially Disappearing

cbenner — Fri, 19 Jan 2018 23:14:26 GMT

Good call! But I wonder still what caused the hole.

Can the dead spot be reproduced on a new drawing from the same template file, or was this a one time fluke error?

Re: Inventor Drawing Dimension Lines Partially Disappearing

Anonymous — Fri, 19 Jan 2018 23:14:41 GMT

it is repeatable from the template.

Re: Inventor Drawing Dimension Lines Partially Disappearing

cbenner — Fri, 19 Jan 2018 23:14:58 GMT

Ok,... try opening the template on it's own. Add a page and delete the first page.... makinmg the new sheet the only one. Save it and then try the drawing again, see if the dead spot is gone for good.

Re: Inventor Drawing Dimension Lines Partially Disappearing

Anonymous — Fri, 19 Jan 2018 23:15:27 GMT

I would think Autodesk would be interested in the files.

Re: Inventor Drawing Dimension Lines Partially Disappearing

VegasRusley — Fri, 19 Jan 2018 23:16:28 GMT

So, is it still my understanding that the only way to resolve this issue, is to copy the views onto another sheet and delete the previous sheet? This is a recurring issue for me and that is the only thing that I have found to resolve it. Does anyone know of a quicker way? I have drawings that have 30-40 parts at times on them and half of the dimensions or leader texts lines disappear and it takes awhile to move everything to a new drawing.

Thanks for any response.

Re: Inventor Drawing Dimension Lines Partially Disappearing

Anonymous — Sat, 20 Jan 2018 00:37:59 GMT

I think I found a fix ,or the reason for the disappearing Dimension leaders. I found I had a text box next to my view that I had dim on and the over lap in the blank space of the text box was causing the leaders to disappear. moving the text box away or changing the size seam to fix the problem.

Re: Inventor Drawing Dimension Lines Partially Disappearing

VegasRusley — Sat, 20 Jan 2018 00:40:44 GMT

I have had instances where your solution is correct, but in the photo that I attached, that is not the case. For some reason, leader lines and dimension lines disappear with nothing around them or interference from each other and the only solution that I have found to correct it is to copy the view on to a new sheet and the leaders will return without issue. Then I must delete the previous dwg sheet and continue on. It's an odd occurrence, but happens frequently.

Re: Inventor Drawing Dimension Lines Partially Disappearing

Anonymous — Sat, 20 Jan 2018 00:41:00 GMT

And you have tried creating a new drawing template? also does it happen in the same location every time?

Re: Inventor Drawing Dimension Lines Partially Disappearing

johnsonshiue — Sat, 20 Jan 2018 14:29:54 GMT

Hi Guys,

I remember seeing this behavior before. This has something to do with hidden layers. The dimension lines are chopped off when there is a text object crossing the dimension lines. It was done as an enhancement quite a few years ago. In this specific case, Go to Annotate tab -> Edit Layers -> turn on "ZN-CGI" layer. You will see the text object. Move it away or delete it and then move the view little bit. It will work correctly now.

If the layer is no longer needed, it should be deleted. Making it invisible is not a good practice, since the objects remain there.

Many thanks!