mirror use and drawing on construction plane

[mbostonsprint]

As I continue to Learn by Doing, I ran across a situation that I found frustrating, but finally solved. The attached screenshot shows a couple of rectangular solids, with holes through them. When I was working on the problem, the rods shown were not engaged in the rectangular parts. Brief summary:

I created the larger block from a sketched centered rectangle, then extruded to size. 

Holes were located per dimension through the extruded thickness onto the initial rectangular face.

Axes were created for the hole centers, as well as a perpendicular/point axis from the center of the rectangular face.

My next intent was to create a smaller thickness rectangular solid on the same axes, with matching cross-section.

I made an offset construction plane at distance from the rectangular face. At this point, I thought I would be able to sketch an identical rectangle on the construction plane, using the construction axes previously created. That was a non-starter, tried several times, and every time the construction plane just disappeared, and the command failed. I gathered from the behavior that sketching on construction planes is impossible.

I then decided to try the mirror command, for the rectangular face only, using the construction plane. That also failed, with an error message stating something regarding one or more pattern elements(?) failed in some fashion.

I ended up having to mirror the body entirely, then split the vertical cylinder from the block, delete the cylinder, and shorten the block to the desired dimension. (Note that I have also changed the vertical cylinder since then; it was previously on top of the block).

So, my questions:

-Is it indeed the case that no sketching is allowed on construction planes? If so, that seems limiting in terms of ease of geometry creation.

-The mirror command seems to have some mysterious characteristics, so where can I find detailed explanantion of its attributes?

Lastly, I note also that there a couple of yellow-boxed items in the timeline at the bottom. This seemed to be an indication of unsaved actions, but I can't figure out how (or whether) that can be corrected, or whether it matters.

Thanks for any help you can offer.

Matt

[joel.palioca]

Hi Matt,

Would you be able to attach the model you are working with so that I can take a look at it?  You can do this by using the export option and choosing archive.  You should then be able to upload here or you can email it to me directly.

In response to your questions here are some points for you.

1. Yes you should be able to sketch on a construction plane.  This is one of the main uses of construction planes is to be able to create geometry on on a plane that isn't on the origin.  Based on what you mention in your post there may be an issue because of the yellow boxes.  If you want to create a quick new design, create a box, and then create a construction offset from a face.  You should then be able to create a sketch on that plane

2. When you mirrored a face what was your intent with it?  Mirroring a face within a body for it to mirror onto will produce an error.  The more common thing would be to mirror the body itself.

3. Yellow-boxed items normally mean that there is a problem with the operation.  This can be caused but a numerous number of things, and this why I am hoping to take a look at the model that you send me.  This way I can help find out what is happening and recommend some fixes for you.

Cheers,

[mbostonsprint]

Joel,

Thanks for the feedback. Model file attached, with some additional work done on it. In response to your questions:

1. OK, I'll try that with some other uncompromised geometry.

2. Mirroring a face just seems like a relatively quicker way to create a similar aligned part using the existing face geometry, and then extrude to a different thickness dimension, especially if the body in question then needs to be highly edited or cut away to get what is required. It seemed more transparent at the time, anyway. 😉

3. Let me know what the errors are (I'm certain there must be some), but more importantly, what the "edit" activity can actually be for these issues. I came up empty on repair methodology, no doubt due to not knowing near enough about how the software can be used.

Thanks

Matt

[joel.palioca]

Hi Matt,

Looking at your file helped give me more information.

I tried creating an offset construction plane and sketching on that plane worked for me.  The one point that I noticed is that this construction plane is beneath the grid which may have led to some confusion. My guess is what happened is that when you created the sketch it kept selecting the grid as the plane to sketch instead of the newly created construction plane.  If you notice behavior like this where it is selecting an object that you don't want and there are multiple objects overlaying each other you can Left click and hold, this will bring up a menu that allows you to select through things.  This way you will be able to select the appropriate geometry.

For the errors that are showing up, it looks like some of the geometry that was used to create the construction point is missing.  Do you know if this point was deleted or something may have happened?  I was able to fix this issue by going back in the timeline and deleting the construction point and then recreating it in the same position.  I think edited the construction axis and used the new point geometry.

For the mirror, it looks like a similar situation where the plane that was used to mirror the object is missing, not sure if it was deleted or what may have happened, but it no longer has a target mirror plane to mirror the body across.  I recreated a construction plane where I believe a plane would have been to get the same result.

See the video below for how I did this.

If you have any information on what may have happened when these errors came up that would be helpful on our end to better understand what is happening.  Also if you did end up deleting the geometry that was used here, understanding what you wanted to delete it is very helpful for us as well.  This way we can help improve the product and reduce these kind of errors happening :).

Cheers,

[mbostonsprint]

Hi, Joel --

Thanks for the info. I believe a major misconception on my part was to think that one would be able to sketch on a construction plane that is oriented isometrically. This doesn't seem possible, unless there is some additional info I don't currently have. I was able to draw on a construction plane when viewed "face-on" (orthogonal view). When I was selecting the (isometric) construction plane in the course of previous action, it was highlighting the plane in the course of the command syntax, but then the construction plane disappeared, and the rest of the command sequence evaporated.

My assumption from what I have discovered with your assistance is that sketching on a construction plane must be done in orthogonal view. It also appears to me that intersection of a construction axis and a construction plane yields nothing usable in terms of selectable points for additional geometry construction on that construction plane. The intersections have no automatic connection to each other; all reference information essentially comes from whatever is seen behind the construction plane. So, a couple of questions:

-Is my conclusion correct?

-Is there any plan to allow isometric view construction plane sketching in future, or is this seen as redundant capability that is otherwise covered? This seems somewhat limiting if that is the case.

With regard to the errors in geometry creation that were in the timeline, I think that this is an indication of need for continued use and familiarization more than anything else. The grid position seems to be an ongoing mystery to me, in that it seems to move to different axial positions relative to the geometry and how it is viewed. I don't have a formulated question here, because I haven't yet gotten an understanding of what affects the displacement of the grid. Probably more on that later --

Thanks again

Matt 

[joel.palioca]

Hi Matt,

So I am going to answer your question based on how I am interpreting it.  When you say you want to be able to sketch on a plane that is isometrically oriented I am guessing you mean you want to be able to sketch on a 2D plane while viewing it from an angle and not "face-on".  If this is the case, yes you should be able to do this.  When you start or edit a sketch it will automatically go to "face-on" since that is the feedback we have gotten from customers is most helpful.

If when you say you want to be able to sketch on a plane that is oriented isometrically you mean you want the capability to do 3D sketching, this is something that we do have.  It is disabled by default, but if you go into your preferences and go to the Design tab there is an option "Allow 3D sketching of lines and splines".  If you enable this it should allow you to sketch in 3D, please note that 3D sketching isn't yet at the capability we would like it to be, hence why it is disabled by default.  This is an area we are looking to improve.

You mention in your post that you were selecting the (isometric) construction plane in the course of a previous action and then the construction plane disappeared as well as ther est of hte command sequence.  I think what you are seeing is the way our timeline operates.  It sounds like when you invoked an action, potentially to edit or make changes to a sketch it rolled back the timeline to the point where the sketch was originally created.  This will step back your model so that the actions that occured after the sketch was originally created haven't happened yet.  If you are looking to make changes based off of future events you can create a new sketch that happens after the construction plane, this way it should still exist for you.

I think I have answered your questions, or maybe I have just made more questions :).  If I am still not understanding or answering you correctly, if you have a video you could show me of what is happening, as well as an example of what you mean by oriented isometrically and being able to sketch this way, it would greatly help me to understand exactly what you mean.

Cheers,