How can I make the following center mark parallel to A line?
Habib Ghalamkari wrote: How can I make the following center mark parallel to A line?
Habib Ghalamkari wrote:
I don't think you can do that with inserted Centermarks. I'd suggest placing sketch lines and adding relations to orient them the way you want. If done properly they will then update if the model changes.
there might be another way, but u could measure angle between centremark and that edhe, and then when u click centremark u can type that angle for it.
But if there's a way of clicking centremark and then choosing to align with edge - that would be great.
thanks for your reply.
I'm aware of this method but every time we have a change in the design of our parts, I have to delete the dimension, measure the angle and
I was looking for a way that could update the drawing in new revisions.
I tried to use something like =RD7*Drawing View4 to make it update with the changes in the design, but SW doesn't accept equations for this field.
Sorry not possible directly but this sounds like a great enhancement. Raise up in the top ten list.
Million thanks to all.
There is I trick you can use. It's a PITA, but will work.
Put in a second hole (can be any size). Just make sure the second hole is aligned with the first hole and parallel to the edge you will eventually want the center mark to be parallel to.
Now put in a Linear Center Mark pattern selecting the two holes.
Next, select and delete the center mark from the "extra" hole.
Go back to your model and delete the "extra" hole.
Will it work if angle changes w.r.t. the edge?
That may work, but wouldn't it be simpler to just place sketched lines instead of the centermark, and define their positions with relations?
I was answering the question as given "How can I make the following center mark parallel to A line?"
I used an actual center mark. I also said it is a PITA.
thanks for explaining your way to do it.
Just to be clear, I would never actually use the technique I described in a real drawing.
I do use Linear Center Marks on almost every drawing I make so I had the insight to know it was possible to use them the way I described.
If I wanted to add a center mark that was rotated, I would sketch draw 2 lines and use relations to orient them.
More likely, I just add the center mark and leave it skewed because that is the fastest way to clearly disseminate the information.
I gave your suggestion a try but...
If you leave the two center marks (the intended one for the hole and the temporary one on the sketch) AND you leave the connecting line between them, then the angle will update as the sketch end is moved around (with a ctrl-Q rebuild). However, if you delete the connecting line between the two points then the angle will NOT update even though the sketch-bound center mark moves as the sketch is modified.
Next I tried leaving both center marks and the connecting line thinking I could move some of them to a hidden layer. Nope, all three entities are selected as a single item. It seems to be all or nothing.\
Per the help file, the Angle shown in the center mark property manager is for feedback ONLY, you can't drive the angle.
HOWEVER, if we flip back from linear center mark to single center mark the Angle setting becomes editable!!!
So I think a method - somewhat tedious - is to figure out the angle either though the measure tool or with some temporary sketch elements and then create a Single Center Point and fill in the angle.
If this is something that you want to do a lot, I would suggest that you make a sketch block for your centre mark, Then by placing this in your design library you can drag it into your drawing view, centre it over the hole and align it with the edge. I think that this would be quicker than drawing lines all the time
Paul thanks for your reply.
I tried your suggestion, but I wasn't able to center the block with the hole or align it to the edge in a view.
After selecting the block ctrl+click the edge doesn't pick anything to make a parallel relation.
Maybe it's because this is my first experience with blocks. What's the trick to do it?
So I have created a part and a drawing, then after placing the drawing view on the drawing I create a center point sketch off to the side of the drawing view.
I then make these lines into a block, then make sure to click on the arrow to the right of "insertion point"
you will now see a message telling you to drag the manipulator to position the insertion point of the block.
Now drag the manipulator to the centre point of the two lines.
then click on the green check mark. you should now have a block
For some reason when I position this block on my drawing view SW will not let me dimension to it. What I have to do is to delete it from the drawing and reinsert it by going "insert block" you can then place it on the centre point of the hole.
Make sure when you have positioned the block that you un-tick the lock angle check box
You will then be able to rotate the block to align with the edge and dimension to it.
If you want to save the block for future use right click on the block and then click on "add to library"
Once you have inserted the first block into your drawing you then either insert another block using the same process or just hold control while you click on the block and drag to the side when you release your mouse button it will have created a copy of the block
Paul I simply don't know how to thank you for taking your time and posting this step by step reply.
I didn't notice that Lock Angle option. Unchecking it solved the problem.
I owe you a hug and two beers.
Once again million thanks.
It's good to know that you got it working. Just one thing to watch out for with using blocks in drawings. Lets say your drawing sheet scale is set to 1:2 and you create the block then you switch to a different drawing sheet or drawing view that has a scale of 1:10 if you insert the block into this drawing sheet the scale of the block will change according to the difference in sheet scales so you might have to resize the block using the scale option just above the lock angle option. Or you could create blocks for each different drawing scale and save them to your library so you use them on your different drawing sheets. You may play around with them a bit using different sheet scales and see what works best for you.
Best of luck
Thanks for additional info.
A few years later, this is still a problem.
You can set the angle for the center mark under its properties. That's what I've done in the past.
Only if the angle is know and a good number.
I need to align the center make to a gear teeth to indicate the location.
I'm sorry my answer doesn't work for the problem you have. =(
I wish it was that simple.
Part of the problem is view is rotated to align with an edge but center mark align to rotated view. Not to sheet.
Frederick Law One approach would be to create a sketch in the gear part with a sketch pattern of circles located where you want your center marks to be - in the middle of each gear tooth. In the drawing view, make the sketch visible. Select the Circular Center Mark option in the center mark tool and pick the sketch circles to define. Then hide the sketch. No angles necessary.
My approach might be something like this:
In the part file create a reference sketch with a circle separated from round boss where you want your center mark. The distance and diameter is immaterial. However, a line connecting the sketch circle and the boss of interest needs to be parallel (or perpendicular) to edge A.
In the drawing view, temporarily set the reference sketch visible. Launch the center mark tool, select the Linear Center Mark option and then select the round boss and the reference sketch circle. This will create two center marks aligned with edge A. Hide the reference sketch. Select and delete the center mark associated with the reference sketch. The round boss center mark will retain its alignment. This method seems to update if the angle of the edge is modified in the model.
I know this is an old post, but there is a way to do this. first pick the edge you want the centerline aligned to, then select the centerline command.
Bob Tosi I am not seeing that behavior in my 2014 version of the software. Perhaps it was added later?
I tried this in 2017 and 2018. It appears to work for center LINES but I didn't get it to work for center MARKS.
I'm running 2018 and it is working for me.
Select an edge:
With the edge selected select your center mark tool:
Select the hole:
Jacob Ziesmer wrote: I'm running 2018 and it is working for me. Select an edge: With the edge selected select your center mark tool: Select the hole:
Jacob Ziesmer wrote:
Doesn't work in 2019 SP2.
In your case, your view is Auxiliary view and all the lines are perpendicular or parallel to each other. Try it in a situation like my view above.
For example a front view that has a slanted bend.
Looks like you are correct. When I initially inserted the center mark it was not properly rotated and the option to manually enter a rotation angle was grayed out. That is what brought me to this thread. I don't know why it works in an auxiliary view and not a standard view.
Retrieving data ...