Houston, We've got a problem?

This forum is for general discussion regarding VCarve Pro
Post Reply
lpcsales
Vectric Craftsman
Posts: 167
Joined: Thu Jul 13, 2006 6:22 pm
Location: NC

Houston, We've got a problem?

Post by lpcsales »

Ok, I've purchased and download a number of the vector3d art's and am trying to incorporate them into a design and I'm beginning to see some problems. Maybe it's me and someone can help. First problem I see is in designing a layout using the designs. I have a basic layout size that I want to incorporate several of the VectorArt3d designs into, but before I can bring them into VCarve Pro, I have to first createa toolpath(s) in Machinist, but to do that I need to know what size to make them.

If I'm in the intial stages of design and placement, I really don't know what size the individual elements will be, so I'm in a catch 22 here. The art files down't come with any sort of placement object file that can first be used in the layout software (Vcarve PRO) so that I can determine what size they should be based upon in my layout.
So how and where do I start a layout using these files as they don't behave like vector art files do in the program? I must be missing something here.

Another problem I found is that I can't copy paste one (any)of the disign elements in the layout. For example, I'm using the corners art file, so I would like 4 of these, one in each corner, in the layout. The only way I have found to get 4 copies of this art file into the layout in VCarve PRo is to do 4 imports...Is this the way it's supposed to work? I notice that the Copy/Paste options are enabled (R-Click) but the actual operation desn't seem to work.

Next, I am having a problem with the rotation.mirroring of the art file, as shown in the picture below crircled in red. I imported the lower right art file and then inported another because I couldn't copy/paste. Next I did a rotation by 90 degrees of the 2nd imported object and it is displayed on the screen as seen in the picture. Something apparently is wrong here. What have I done wrong on this? Note, however, that when the program generates a preview of the toolpaths, it does show it correctly.

also, is there anyway for the program to display guide lines? It would be really helpful when you need to align mutliple objects on a common dimension?

I'm sure I'm doing something really stupid here, so please, if anyone can help me Iwould really appreciate it.

Thanks
Attachments
new-1.jpg
(149.67 KiB) Downloaded 161 times
Dave
Epilog 24TT 40w and Legend 36EXT 75w Laser Engravers, Roland SP-300V, BabyLoc PR600 Embroidery Machine, Panther 24" Vinyl Cutter, Mighty Presses (hat & T-Shirt), PRT48 Router

lpcsales
Vectric Craftsman
Posts: 167
Joined: Thu Jul 13, 2006 6:22 pm
Location: NC

Post by lpcsales »

To further this along... I mentioned previously that the preview looked ok, but... I added a rectangle border so I could creat a pocket, assigned a .25 dia. end mill to the toolpath and did a preview all toolpaths (reset preview 1st) and the picture below shows what I'm getting as the output. I don't know whether to trust this or not. Haven't run the project yet, but I have found that what you see in the preview is pretty much what you will see in the final results.

The problem is circled in RED and leads me to believe that it is associated with the copy/paste problem I mentioned above. I can't find a way to get this out. Has anyone found a workaround?
Attachments
new-4.jpg
(230 KiB) Downloaded 149 times
Dave
Epilog 24TT 40w and Legend 36EXT 75w Laser Engravers, Roland SP-300V, BabyLoc PR600 Embroidery Machine, Panther 24" Vinyl Cutter, Mighty Presses (hat & T-Shirt), PRT48 Router

lpcsales
Vectric Craftsman
Posts: 167
Joined: Thu Jul 13, 2006 6:22 pm
Location: NC

Post by lpcsales »

Sorry about all this posting...but I have found an area that could be a problem, especially when generating your toolpaths.

If you have several objects in your design and the toolpaths have been generated then you go to the design stage of the program and delete any or all of the objects, the toopaths are left behind as ghosts. As an example from the above posts, in trying to correct the problem with the 2 far right corner objects, I deleted them from the designer side, when I go to the toolpath side, the previously generated toolpaths still exist. Now because all 4 objects were multiple imports of the same object, they carry the same toolpath names. This is quite confusing when I want to try and save the toolpaths to a cut file...which one is for which?

It seems to me that if you delete an object in the design that the toolpath for it should also be deleted, maybe with a warning that this is going to happen. Otherwise you are left with a ghost. It looks like there is no linking of objects to associated toolpaths.

Does this make sense?

...or am I working too late into the evening :oops:
Dave
Epilog 24TT 40w and Legend 36EXT 75w Laser Engravers, Roland SP-300V, BabyLoc PR600 Embroidery Machine, Panther 24" Vinyl Cutter, Mighty Presses (hat & T-Shirt), PRT48 Router

User avatar
Tony Mac
Vectric Alumni
Posts: 1985
Joined: Sat Jul 30, 2005 6:24 pm
Location: UK
Contact:

Post by Tony Mac »

Hi Dave,

It looks like you had a frustrating evening.

I'll create a Video Tutorial showing how to combine VA3D designs with VCPro jobs. But it's also worth looking at some of the points so you have a better idea of how this integration works.

1. Sizing VA3D designs
The easiest way to determine what size the toolpaths for the3D design need to be is to layout your design in VCarve Pro and draw rectangle to represent the size and position of the 3D toolpaths. Make a note of the size of the rectangles (size of the elected vector(s) is displayed in the bottom right corner of the screen) and use these dimensions in the VA3D Machinist software.

Drawing the rectangle is also very useful for positioning the 3D toolpaths.
Select the grayscale preview hold the Shift key and select a corner rectangle then click the Align option Center Vectors. This moves the grayscale preview + associated 3D toolpath to position of the selected rectangle.

I guess that you would like to size / stretch the grayscale preview + 3D toolpath inside VCPro. This isn't possible because the toolpath has to be calculated for a specific job size, cutter size and stepover to produce the required surface finish. Stretching or resizing a design in VCPro would result in the surface finish changing due to the stepove being stretched.

2. Copy Paste
This is done using the Copy Toolpath option on the Toolpath Operations list

This creates a copy of the selected VA3D Toolpath that can then be moved (to another corner in your example).

3. Rotation
The selected grayscale preview can be mirrored and flipped and the associated toolpath also gets transformed to the same orientation.

Rotating toolpaths by an arbitrary angle is not supported and we will ensure these options are greyed out in future versions to avoid confusion.

For your corner pieces I would suggest using the Mirror command to flip the design into the required orientation .

4. Guidelines
This feature has been requested and is on the development list. In the mean time the best work around is to again draw rectangles and use the auto alignment options to position objects relative to an edge or middle. This is not a perfect solution but can be used for accurate positioning.

5. Toolpath Preview
Not sure why the preview image looks incorrect but possibly down to having deleted the grayscale preview for a toolpath in the 2D window but left the actual toolpath?

Using Toolpath Copy to add multiple copies of a 3D toolpath should help with this.

6. Deleting imported 3D Toolpaths
When deleting a 3D Toolpath the 2D grayscale image also has to be deleted and vice-versa. This will delete the ghost objects.

Good idea for a future enhancement that would be to link these 2 objects so they both go when one is deleted. This has been added to the enhancement list.

7. Renaming 3D Toolpaths
Double clicking on a 3D toolpath name in the list or using Edit Toolpath opens a form that allows the toolpath to be renamed to make it more meaningful.

This for is also very useful for positioning the 3D toolpath into the material (in z). The VA3D Machinist software positions the toolpaths relative to the material surface / base. The Editing form allows the toolpath to be moved in the Z axis.

For example to place the 3D carving inside a 0.5" deep pocket.
Double click / edit the 3D toolpath and change the Start Depth = 0.5"

It's also worth noting that the speeds, feedrates and tool number can be edited inside VCPro without having to go back into the VA3D Machinist software. The Cut Depth cannot be changed as this is preset when the original toolpath + size, cutter and stepover were specified.


I hope this all makes sense and I'll look at putting a video together to cover these points.

Tony

User avatar
Les_linton
Vectric Craftsman
Posts: 148
Joined: Sun May 28, 2006 5:52 pm
Model of CNC Machine: ViperX7
Location: Pekin, IL

Post by Les_linton »

Hey Dave,

Tony has addressed most of the issues that you had connected with this problem.

While I think Pro and Machinist are great programs, I am more comfortable in AutoCad so I use that to do my basic design work at this time. Sometime it is very primitive, but it works for me.

I lay out my basic piece to size and them simply draw the carving as ovals, circles or corners (detail is not important yet) and scale and position with the tools I'm comfortable with. Once I know that information I can use Machinist to size my parts. I can then import the basic shape of the project into Pro as a dxf, and then import my toolpaths from Machinist and place them according to my concept drawing.

It sounds cumbersome, and sometimes is, but then you read the forum and what others are doing and you will often do a "damn, I didn't know I could do that" and move onto easier ways.

In the mean time, get a wood stove and keep practicing...

Les

lpcsales
Vectric Craftsman
Posts: 167
Joined: Thu Jul 13, 2006 6:22 pm
Location: NC

Post by lpcsales »

Hey Tony, Thanks very much for the very helpful input. I did have a rough evening and never did get the disign completed. Don't get me wrong, you do have some great software and I wouldn't want to be without it. Keep up the good work.

Normally, I do my layouts in CorelDraw X3, similar to what Les is doing. I'm real comfortable with that program and it does an exacting job. This particular design, I was using the 3D art for the first time and figured it should be layed out in VC Pro instead, so there I was, along with the problems I encountered.

I think that what I will do now is to take the bitmap of the 3D file and give it a quick trace in CorelDraw to get a simple outline of the figure. When I'm doing a design layout I need to see at least the shape of the item I'm placing down, it helps me tremendously, especially when bringing multiple elements together into one. So with an outline of the art file on screen in CorelDraw, I can quickly do my layout design. When done I'll know exactly what size each 3d art image should be and I can then move into 3D machinist and so on.
Thanks again all!

A quick question for Tony...
In my original example on this thread, regarding the 4 corner elements that are all just copies of 1, is there anyway, being that they will be using the same tooling, feeds, etc., to group the 4 elements together and create just one toolpath instead of 4 ea., ie., 1 for each of the roughing and finishing? I was thinking that if the 4 elements were each selected, then grouped, then the toolpaths could also become one instead of 4. I know this would not work if the elements were different, using different tooling etc., but, wow, it would be nice if you only had to deal with one cut file verses 4, etc. in situations as this. :roll:

Just some wishful thinking...

All the best,
Dave
Epilog 24TT 40w and Legend 36EXT 75w Laser Engravers, Roland SP-300V, BabyLoc PR600 Embroidery Machine, Panther 24" Vinyl Cutter, Mighty Presses (hat & T-Shirt), PRT48 Router

User avatar
Les_linton
Vectric Craftsman
Posts: 148
Joined: Sun May 28, 2006 5:52 pm
Model of CNC Machine: ViperX7
Location: Pekin, IL

Post by Les_linton »

Dave,

Once you have all of your 3D toolpaths placed, when you go to "save toolpaths" move all of your roughing toolpaths to the save side and save them as one file, then do the same for your finishing toolpaths.

When you run the files they should all cut at the same time. I did eight of the same file on one piece, and the only issue I had was that I got a couple out of order so instead of cutting 1 through 8 it cut 1, 3, 4, 2 and so on. My mistake..

Good luck.

Les

Paul Z
Vectric Wizard
Posts: 517
Joined: Sun Apr 30, 2006 10:04 pm
Model of CNC Machine: shopbot PRT Alpha 96x48
Location: New Hampshire, USA
Contact:

Post by Paul Z »

I thought the arrows on the toolpath list were scroll arrows until I needed to reorder the toolpaths one day. I finally figured out that they were reordering arrows. Have you ever felt really smart and really stupid at the same time?

Paul Z

User avatar
Les_linton
Vectric Craftsman
Posts: 148
Joined: Sun May 28, 2006 5:52 pm
Model of CNC Machine: ViperX7
Location: Pekin, IL

Post by Les_linton »

Paul,

I couldn't figure out why they weren't moving when I scrolled down.... :roll:

Glad I wasn't the only one...

Les

lpcsales
Vectric Craftsman
Posts: 167
Joined: Thu Jul 13, 2006 6:22 pm
Location: NC

Post by lpcsales »

Les, you know, the last time I tried to save multiple toolpaths to a single file, I got the message that my post processor didn't support tool changes....so have never messed with it since. But, I never thought about it for this application as there are no toolchanges, they would all be the same.

Ooooh! I'm glad you are around Les. Thanks!
Dave
Epilog 24TT 40w and Legend 36EXT 75w Laser Engravers, Roland SP-300V, BabyLoc PR600 Embroidery Machine, Panther 24" Vinyl Cutter, Mighty Presses (hat & T-Shirt), PRT48 Router

User avatar
Les_linton
Vectric Craftsman
Posts: 148
Joined: Sun May 28, 2006 5:52 pm
Model of CNC Machine: ViperX7
Location: Pekin, IL

Post by Les_linton »

Same issue here Dave. On the 3D stuff you have to save Roughing and Finishing seperate.

It's not that I'm any smarter Dave..... I just made the mistake sooner!!! :lol:

Les

Post Reply