Have a few quick questions about dimensions in the drawing space

[damiennn_w]

Hi, I'm trying to dimension along the arc of a tube to the center of a pin, it's how it would be done in the workshop, but I'm having real trouble doing that, it will give me the overall arc length but I just can't seem to find a way to show where the pins go other than using an aligned measurement. I've previously been shown how to use the section view to dimension arc lengths that aren't complete, but it doesn't work for this. Iv'e attached a quick example model in the hopes that someone can please show me how to do it. So from the end of the tube, along the outside arc of the tube to the center of each pin, Thanks in advance.

[jhackney1972]

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@damiennn_w wrote:

 So from the end of the tube, along the outside arc of the tube to the center of each pin, Thanks in advance.

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The last sentence mentions the Outside Arc of the tube but to me this is a useless edge.  I did the Arc dimensions from each pin on the centerline of the arc.  I can create the arcs lengths to the edge you specify if you really mean to use it.  Model is attached the drawing came from.  Note the Sketch labeled Arc Length Sketch.

[damiennn_w]

Thank you, I knew you would know how to do that, but yes the out side arc is the one that would be used in a fabrication shop, since you can't run a tape measure on the centre of the tube, only the outside curve can be measured in real terms. On larger tubes the difference between those centre and external lengths will matter more than with that small diameter tube, I just wanted to know how to do it as it's quite a common thing to have to dimension in my line of work. Is it done the same way as you showed me before, i.e with the section view first? I ask as it wasn't working for me, but my fusion has been crashing every ten minutes so maybe that is why it wouldn't work for me. 

There is one more similar dimension I haven't been able to do also, I'll have to draw a quick model again as an example to try to explain it properly if you wouldn't mind showing me how to do that too? 

[damiennn_w]

Having looked at the sketch you mentioned, does that mean that to get the result the sketch has to be added in the design space then used in the drawing space? Sorry if that is a silly question I'm just really not sure how you did it 😀

I've attached another that I was having trouble with, I need the same outside arc measurement from one of the ends of square tubing to the center of the intermediate pieces, for the same reason as before, to accurately place those crosspieces the tape measure has to run along the external arc, either that or an aligned measurement to one of the corners instead, but in my opinion it doesn't look as professional when done that way, and it can't always be achieved if other section of steel are in the way which has been known to happen in some designs.

[jhackney1972 · Accepted solution]

Yes, I create a separate sketch in the model environment and added Center Point Arcs for each segment.  I then turn on this sketch in the drawing environment and use the Arc Length command to label them.  Sometimes you need to toggle the visibility of the sketch in the drawing environment off and on to make the Arc Length command pick it up.  The model for the corrected foot placement to the outside arc of the tube and the model for the cross member location by arc length on the outside wall of the tube are attached.  Look for the labeled sketches in each.

[damiennn_w]

That's great, than you for your all your help!

[damiennn_w]

Hi, sorry to bother you again, but I'm finding it very hard to create the result on my model that you got with the tube sample I posted originally. I added the separate sketch and created points on the outside of the tube. But as I've now tried to show that in the drawing space to use for the dimensions, nothing is showing, After doing the section view I just get the overall arc length of the part and still can't show the placement of the pins. I've checked that the sketch is visible but it doesn't show on the part at all. Any idea what I'm doing wrong? Does the sketch have to be in the same sub assembly as the part?

Also, I tried to save just the sub assembly to f3d format to post on here, saving it worked fine, but when I opened it in fusion to check it had worked, all of the pins and base plates where all over the place rather than in there correct positions attached to the tube. Does fusion not export the joints or patterns with the model or did I do something wrong? Even the sketches where in the wrong place also.

[jhackney1972]

Fusion will export an assembly or sub-assembly and retain joints.  I do not know how you broke up your assembly so I cannot say why you had difficulty when you opened your export in Fusion.  If you want to export the complete assembly I will take a look. 

Below is the video on the process of placing the arc lengths on the drawing.  I used your original rail and posts.  Please note that sometimes you may have to toggle your sketch on and off to make it available for dimensioning.

[damiennn_w]

Thank you so much for taking the time to do that for me, I had missed using the intersect command and had offset the centre line instead in my model, I'm always impressed at how easy this stuff is for you. I really appreciate the work you put in on here, 

As for the model breaking when exported, I'm really not sure what I did wrong when modelling it, I used joints on the first leg and baseplate I added, then created the pattern on path, then made a rigid group of the whole foot rail. But after re-importing the saved version they were all over the page, I'll have to try and be more disciplined with the method I model with from now on and try to avoid it happening again. If on another model it does repeat I'll send it over to you for you to take a gander, if you don't mind that is. But thank you again for showing me how to get those arc lengths.