I have sketched a square with overlapping circles located near each corner. The eventual purpose of the circles is to make an outer radius corner so that a square object will fit into the square shape. I initially had trouble trimming away the parts of the square that were inside the circles, but altering the order of which segments and circles were operated on got me past that. So that is one bug. Another bug that I cannot seem to work around is that the parts of the circles that are fully inside the square can be selected in the trim operation but never get trimmed. Has anyone found out the correct procedure for trimming part of a circle where it intersects another shape?
JST
Alibre Super User
I have found that to be FAR better than a sketch feature prior to extruding.
For one thing, you can edit it very easily, which is a big plus.
For another thing, sketches are best kept as simple as possible. The fancier a sketch is, the harder it is to edit, and the more you lose if something gets fouled up.
For one thing, you can edit it very easily, which is a big plus.
For another thing, sketches are best kept as simple as possible. The fancier a sketch is, the harder it is to edit, and the more you lose if something gets fouled up.
Harold:
Actually, I had originally tried doing it that way but Alibre refused the operation of extruding the circles after extruding the square, so I decided to try to create the composite shape and do a single extrusion instead. The Alibre original refusal claimed that the shapes were not closed. I took that complaint to mean that it did not like removing material on the inside of the square where no material existed since the previous extruded squared had already remove it.
Also previously unstated is that I need to perform this material removal 12 times in a circular pattern, which made creating a composite shape to begin with the obviously more attractive (but apparently unworkable) approach. This method should be workable since it is so obvious.
I just thought of another approach that I could try. I could try to create a composite solid part (all additive) and then use the Boolean operations to subtract that part from the solid disk.
Actually, I had originally tried doing it that way but Alibre refused the operation of extruding the circles after extruding the square, so I decided to try to create the composite shape and do a single extrusion instead. The Alibre original refusal claimed that the shapes were not closed. I took that complaint to mean that it did not like removing material on the inside of the square where no material existed since the previous extruded squared had already remove it.
Also previously unstated is that I need to perform this material removal 12 times in a circular pattern, which made creating a composite shape to begin with the obviously more attractive (but apparently unworkable) approach. This method should be workable since it is so obvious.
I just thought of another approach that I could try. I could try to create a composite solid part (all additive) and then use the Boolean operations to subtract that part from the solid disk.
HaroldL
Alibre Super User
Hmmm...using the Boolean operation could get messy too. Are you planning to do a Boolean Subtract for each instance?
If Alibre is warning of an open sketch then use the Sketch Analyze tool to show where the open is an maybe correct it. IF the gap is too great at least it will indicate where the problem is so you can edit it manually.
Once you get one of the cutouts done you can then use the Circular Feature Pattern to make the remaining instances -- as long as rotation is allowed for each. I have seen some parts that all instances of the circular patterns had to be aligned. THAT is not possible in Alibre - (yet?)
You didn't mention any dimensions but I guesstimated a disc part with 12 cutouts as an example of a workflow. If you edit the dimensions of the circles at Extrusion<2>, the cutout, Extrusion<3>, will follow when you rebuild the part.
If you can share an example it may be more clear what your issues are and give better advice.
If Alibre is warning of an open sketch then use the Sketch Analyze tool to show where the open is an maybe correct it. IF the gap is too great at least it will indicate where the problem is so you can edit it manually.
Once you get one of the cutouts done you can then use the Circular Feature Pattern to make the remaining instances -- as long as rotation is allowed for each. I have seen some parts that all instances of the circular patterns had to be aligned. THAT is not possible in Alibre - (yet?)
You didn't mention any dimensions but I guesstimated a disc part with 12 cutouts as an example of a workflow. If you edit the dimensions of the circles at Extrusion<2>, the cutout, Extrusion<3>, will follow when you rebuild the part.
If you can share an example it may be more clear what your issues are and give better advice.
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JST
Alibre Super User
Hold the 'phone.......
You said you had overlapping circles in the sketch for removing material on the corner. You have to make each extruded shape a SINGLE outline, by removing interior lines.
Not doing that will give errors. A mistake in removing lines may give a non-closed shape. The problem with the extrude cut may be something of that nature.
You said you had overlapping circles in the sketch for removing material on the corner. You have to make each extruded shape a SINGLE outline, by removing interior lines.
Not doing that will give errors. A mistake in removing lines may give a non-closed shape. The problem with the extrude cut may be something of that nature.
bigseb
Alibre Super User
i have seen this issue many times. Sometimes two interesecting sketch features just wouldn't trim. Even on simple stuff like Zetopan mentions. When this does occur no amount of fixing/redrawing works. You have to kill the entire part and start from scratch. A MASSIVE time suck. Also looks bad when the boss is peering over my shoulder..
There is validity for doing this in one sketch as opposed to the preferred method of breaking the process up into two or more steps namely that it leave only one step in the design tree. And lets be honest, this is still a relatively simple feature i.e. a square extrude cut with clearance corners. There shouldn't be any reason why this should cause Alibre to fall over if doing it in one go.
There is validity for doing this in one sketch as opposed to the preferred method of breaking the process up into two or more steps namely that it leave only one step in the design tree. And lets be honest, this is still a relatively simple feature i.e. a square extrude cut with clearance corners. There shouldn't be any reason why this should cause Alibre to fall over if doing it in one go.
Thanks for the suggestions everyone, I finally got it to work using the method that HaroldL suggested. I fully agree with bigseb that this should easily work using a 2D sketch. The odd thing is that when I do a trim it correctly identifies the circular arc that is to be trimmed, but simply refuses to remove it with no error message or anything else. Using Assembly Booleans also did not work. I could bring in the part and place it correctly, but the "tool" could never be subtracted from the "blank" like the user's manual describes this operation. As a result I had to create a square and extrude it into the blank and then follow that up with four circles being extruded into the same blank. Circular replication of that resulting negative extrusion then created the desired result in the blank. Seems to be a lot of things currently broken in Alibre.
oldfox
Alibre Super User
Personally, I have never had any problems with "trim figure" that I couldn't explain.
Seb, I use both of the methods you mention. If I am real comfortable with what I am doing, I will put everything
in one sketch. If, however, I'm trying something I may not be that familiar with, I'll save the file and then start a new
sketch in case anything breaks. That way, as you say, there is much less to re-do.
Zetopan, load up the sketch below and you can play with it. "Trim Figure" is really one of the basic features of AD.
What version of AD/GD are you using?
Now let me explain the sketch. The top 2 circles are really *4* circles. 2 upper left superimposed and 2 upper
right superimposed. The 2 bottom circles are single circles. Notice the dots at about 12:30 on the upper circles.
That is an indicator that there are more than one. It may also mean something more that I'm not aware of.
Next, notice that the upper right circle has 2 "points" on the rectangle lines. Those are *true trim end points*
of one of the circles. What you are seeing as a "non-trimmed" circle is the underlying circle. If you subsequently
trim that portion again...
Voila!! There's the problem.
And of course, the lower left is all single figures trimmed as you desire.
Hope this helps. I'm guessing, possibly very wrongly, that you haven't been using Alibre very long. Just an innocent
assumption.
-oldfox-
Seb, I use both of the methods you mention. If I am real comfortable with what I am doing, I will put everything
in one sketch. If, however, I'm trying something I may not be that familiar with, I'll save the file and then start a new
sketch in case anything breaks. That way, as you say, there is much less to re-do.
Zetopan, load up the sketch below and you can play with it. "Trim Figure" is really one of the basic features of AD.
What version of AD/GD are you using?
Now let me explain the sketch. The top 2 circles are really *4* circles. 2 upper left superimposed and 2 upper
right superimposed. The 2 bottom circles are single circles. Notice the dots at about 12:30 on the upper circles.
That is an indicator that there are more than one. It may also mean something more that I'm not aware of.
Next, notice that the upper right circle has 2 "points" on the rectangle lines. Those are *true trim end points*
of one of the circles. What you are seeing as a "non-trimmed" circle is the underlying circle. If you subsequently
trim that portion again...
Voila!! There's the problem.
And of course, the lower left is all single figures trimmed as you desire.
Hope this helps. I'm guessing, possibly very wrongly, that you haven't been using Alibre very long. Just an innocent
assumption.
-oldfox-
dwc
Alibre Super User
I have very very rarely seen similar behaviour. My solution has been to save the part and then close and restart AD. After that it works again. Something must be getting messed up internally. It happens so rarely that I have not spent the time to see if it is because something is messed up in the part, that reloading solves, or if it is because AD is restarted.
Don
simonb65
Alibre Super User
I've had quite a few occurances recently of not being able to trim or extend. I had to resort to deleting the sketch lines, arc and circles that wouldn't respond and redraw them! There isn't a repeatable way to reproduce this, but for the developers you can work backwards from what is needed for the trim and extrude to work and find out what piece of data or status of the sketch item would be wrong for this not to happen ... and then look in the code for what may not be setting that correctly!
oldfox said:
"Zetopan, load up the sketch below and you can play with it. "Trim Figure" is really one of the basic features of AD."
I cannot load that part since you are using a newer version of Alibre.
What version of AD/GD are you using?"
I am using Alibre 2017. I am considering upgrading to maintenance for 2017, which is likely what you are using.
"I'm guessing, possibly very wrongly, that you haven't been using Alibre very long."
I have been using Alibre for several years. I started so many years ago that I do not recall the starting version (it was named Alibre at the time, well before the Geomagic mess). However, the particular features that I recently attempted to use are new to me since I had not used them before now.
I generated the geometry with a new sketch that only included a single square and one round shape near one corner. Alibre refused to let me save that as a file since it generated errors when I tried to save. So I deleted the round shape and used a circle instead. The circle and the square corner trimmed perfectly, while the round shape and the square corner did not. So I assume that this is basically a pilot error, although I do not know why a round shape (which was my preferred method of sketching since it specifies the diameter) gets treated any differently than a circle for trimming intersection purposes.
And I want to thank the Alibre user community for being so responsive to my request for assistance.
"Zetopan, load up the sketch below and you can play with it. "Trim Figure" is really one of the basic features of AD."
I cannot load that part since you are using a newer version of Alibre.
What version of AD/GD are you using?"
I am using Alibre 2017. I am considering upgrading to maintenance for 2017, which is likely what you are using.
"I'm guessing, possibly very wrongly, that you haven't been using Alibre very long."
I have been using Alibre for several years. I started so many years ago that I do not recall the starting version (it was named Alibre at the time, well before the Geomagic mess). However, the particular features that I recently attempted to use are new to me since I had not used them before now.
I generated the geometry with a new sketch that only included a single square and one round shape near one corner. Alibre refused to let me save that as a file since it generated errors when I tried to save. So I deleted the round shape and used a circle instead. The circle and the square corner trimmed perfectly, while the round shape and the square corner did not. So I assume that this is basically a pilot error, although I do not know why a round shape (which was my preferred method of sketching since it specifies the diameter) gets treated any differently than a circle for trimming intersection purposes.
And I want to thank the Alibre user community for being so responsive to my request for assistance.
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simonb65
Alibre Super User
Can you post a picture (screen snip) of the sketch that wouldnt trim.
simonb65 said:
Can you post a picture (screen snip) of the sketch that wouldn't trim.
Sure thing, see the attached JPG file. The square shape is 0.3150" on a side. The round shape has a diameter of 0.0625" and its center is located 20 mils inside the top and left sides of the square. This cannot be saved in a file and it also cannot be trimmed. Specifying a circle instead of a round shape allows trimming.
Can you post a picture (screen snip) of the sketch that wouldn't trim.
Sure thing, see the attached JPG file. The square shape is 0.3150" on a side. The round shape has a diameter of 0.0625" and its center is located 20 mils inside the top and left sides of the square. This cannot be saved in a file and it also cannot be trimmed. Specifying a circle instead of a round shape allows trimming.
Attachments
oldfox
Alibre Super User
Zeto, I use Alibre very simply. So a lot of things I hear or read don't make a lot of sense to me sometimes. I hate
to say it, but this is one of those times. Looking at "Noname.jpg" I see a square and a circle. What do you mean by
"round shape". I only use circles, arcs and ellipses.
I drew the sketch and could not make "Trim Figure" fail. It trimmed anything I wanted. I did use a "circle". Tell me
what you mean by round shape and I'll try that.
Oh, btw, I am using 2017.1
to say it, but this is one of those times. Looking at "Noname.jpg" I see a square and a circle. What do you mean by
"round shape". I only use circles, arcs and ellipses.
I drew the sketch and could not make "Trim Figure" fail. It trimmed anything I wanted. I did use a "circle". Tell me
what you mean by round shape and I'll try that.
Oh, btw, I am using 2017.1
JST
Alibre Super User
Oldfox....
If he is making a sketch with overlapping circles that need to be converted to one outline by deleting lines, and then are extruded, its a bit of work to do or edit that. Worth doing a separate sketch and extrude for one, and a pattern to do the other 3 if possible.
If he only means to overlap a single circle onto each corner, then it does not matter much how it is done. The description and illustration seemed not to be the same, description was not clear to me.
Patterns are usually easier to edit, as you only do the original shape once.
If he is making a sketch with overlapping circles that need to be converted to one outline by deleting lines, and then are extruded, its a bit of work to do or edit that. Worth doing a separate sketch and extrude for one, and a pattern to do the other 3 if possible.
If he only means to overlap a single circle onto each corner, then it does not matter much how it is done. The description and illustration seemed not to be the same, description was not clear to me.
Patterns are usually easier to edit, as you only do the original shape once.
oldfox
Alibre Super User
JST,
Once I have my locations established, I just draw one circle, dimension it and draw 3 more that snap to the first one's
dimension. Then I trim out the lines and inner curves and I'm done. Never had to go to another sketch, just extrude
what I had. That, for me, is less work than doing multiple sketches. Do you pattern the sketch figures or the solid object?
Once I have my locations established, I just draw one circle, dimension it and draw 3 more that snap to the first one's
dimension. Then I trim out the lines and inner curves and I'm done. Never had to go to another sketch, just extrude
what I had. That, for me, is less work than doing multiple sketches. Do you pattern the sketch figures or the solid object?