Getting Accurate Dimensions from an Isometric View?

[DraftingNMS]

I am trying to use a single isometric view to show simple dimensions. I am able to get dimensions that look good, but their numbers are wrong. I know I can manually overwrite the wrong number and replace it with user text, but I find it bad practice to do that.

Example: a 10" gap in the model is measured as 8-3/16" on the isometric view.

How do I get it to measure it as 10"?

[Cary OConnor]

Is the view set to True Iso Dimensions on the View Properties? Can you send the simple example and we can look at it?

[Malcolm Crowe]

There are a couple of things to keep in mind when dimensioning isometric views:

1. Set View Properties\Dimensions to "True" (as opposed to projected used for orthographic views). See attached image.

2. This is the less obvious point, but is important. Select one edge for the first point (to define the direction of the extension lines), followed by one vertex for the second point. Then the dimension line position. See the attached video.

Malcolm

[DraftingNMS]

From what I can tell, the view is set to "Create True Iso Dimensions". It does give me accurate readings when I measure the length, width and height of the part, but the distance between two bolt patterns are incorrect, regardless of whether I use centerlines, center marks, or no annotation at all.

EDIT: I forgot to delete all the unnecessary numbers, but the key one to go for is located near the text "DETAIL:C".

IsoIssue.icdC-2.5x2.5x0.3125-CUBA-R5.ics

Edited December 4, 2020 by DraftingNMS

[Malcolm Crowe]

I can see your problem dimensioning those holes. Sorry, but I don't know what the solution is in ICD.

Malcolm

[Cary OConnor]

Hmm.. I see it as well. We need to file that to see what could be the case. 

One way around it is to go to the 3D and place the dimension. Set the dimension to transfer and it will show the correct value in the ISO View. 

[Malcolm Crowe]

The hole distance dimensions correctly in CAXA.

[DraftingNMS]

The dimension transfer function does what I need it to. Not as quick a process as the usual dimensioning, but it does the job while looking normal.

I have no experience with the CAXA drawing space. What sets it aside from the normal drawing space?

 

My guess on the issue may not be worth much, but here it is: I think that the software for this drawing environment makes dimensions based off of line info, and if a line is not explicitly available, it uses point-to-point info based on the sheet. It's accurate when the view is facing the viewer directly, but flawed when it is not direct, like an iso view. I took a direct view of a 8-3/16" block, lined it up with the iso view, and it looks like an exact match.

EDIT: I have feeling this is issue is just the nature of the normal 2D drawing space, and not something that could be fixed.

Edited December 4, 2020 by DraftingNMS

[Malcolm Crowe]

Regarding CAXA, it is more versatile than ICD; with more drafting tools. It is a genuine 2D DWG Editor (like AUTOCAD etc....).

If you need to collaborate with clients or suppliers using DWG and DXF files, or if you want to share Annotation Blocks, Symbols, etc.... with other CAD software, then this is what you should be using. If your drawings are only ever used inhouse (with no need to collaborate outside), then it is a matter of personal preference whether you use ICD or CAXA. Although, having said that, I would recommend CAXA (IRONCAD DRAFT) to Managers of large design offices.

Malcolm

[GNÄSLUND]

Do CAXA drawing dimensions associate with the model so changes to the model will propagate to the dimensions?

[Malcolm Crowe]

Yes. If the 3D model changes the generated views and associated dimensions in CAXA will change also.

Malcolm

[DraftingNMS]

I thought I was done with questions, but now I have another.

I have pulled three dimensions from the drawing I am doing that are horizontal. One of them need to be vertical. How do I reorient it?

[Malcolm Crowe]

Have you tried point 2 of my original post ? Or are you dimensioning holes?

On 12/5/2020 at 8:59 AM, Malcolm Crowe said:

2. This is the less obvious point, but is important. Select one edge for the first point (to define the direction of the extension lines), followed by one vertex for the second point. Then the dimension line position. See the attached video.

Malcolm

[Cary OConnor]

If you are looking to reorient, you can do it during creation by right-clicking or hitting tab to toggle H,V, and Parallel. If it is already placed, right-click on the dimension and there is a reorient menu option available to adjust it. 

[DraftingNMS]

Can you screenshot what you mean? Something on my end is not adding up.

[Cary OConnor]

Sorry I was referring to the ICD dimensions. 

For the 3D, the only way I found to do this is to move the dimension back to the original location (so the arrows are at the points). Rotate your view to the orientation you would want to pull the dimension in. Then pull in that direction and it should allow you to change from say horizontal to the vertical placement. 

 

[DraftingNMS]

I can do that now, but probably because of the model, it is a royal pain to get it right the first time.

Is there a way of doing it in the white drawing space for a dimension I transferred from the 3D space? I couldn't find an option to do that.

[Cary OConnor]

I don't see a way to change it on a transferred dimension. We will need to file an ER for it.