Merry Christmas - Free Designs

This forum is for general discussion regarding VCarve Pro
User avatar
Tony Mac
Vectric Alumni
Posts: 1965
Joined: Sat Jul 30, 2005 6:24 pm
Location: UK
Contact:

Merry Christmas - Free Designs

Post by Tony Mac »

We have put together some Festive Christmas designs that can be downloaded and machined using both the Full and Trial Versions of VCW 2.0.

Click on the link below to visit the web page where you can downoad the files, tutorial videos and pdf manuals.

Image

Free Christmas Designs

If you would like to cut these designs but don't have the software, download the Free Trial Versionand this will allow the toolpaths to be saved, so you can run them on your own CNC machine.

If you have any questions about working with these files or need our assistance please e-mail - support@vectric.com

Tony
Attachments
Decoration2.jpg
Christmas decoration
(153.07 KiB) Downloaded 396 times
Last edited by Tony Mac on Sun Oct 22, 2006 9:26 pm, edited 1 time in total.

User avatar
Uncle Hai
Vectric Craftsman
Posts: 117
Joined: Thu Sep 22, 2005 3:32 pm
Location: Herndon, VA -USA
Contact:

Post by Uncle Hai »

It's nice of you to bring this project up to share with everyone, that is nice holiday spirit of you!
Keep it up. Thanks Tony,
There is something wrong with my screen or VCW software I couldn't delete waste material like you did.
Can you tell what is wrong?( this is original file downloaded from yours, no alteration)
Regards,
Attachments
Santa+sleigh.jpg
(155.62 KiB) Downloaded 388 times

User avatar
Tony Mac
Vectric Alumni
Posts: 1965
Joined: Sat Jul 30, 2005 6:24 pm
Location: UK
Contact:

Post by Tony Mac »

Hello Uncle Hai,

Very nice to hear from and I hope all is well on your side of the 'pond'.

Afraid the Delete Waste Material cannot determine that the inner regions of this design should be removed, it works from the outside border until it finds the gaps created by the toolpath.

The 'Trick' for creating a more realistic image of the fnished piece is to simply calculate a 2D Pocket Toolpath and then Preview the results - see the atached file.

Hope this helps,

Tony Mac
Attachments
Santa_Sleigh_Pockets.zip
(386.6 KiB) Downloaded 321 times

User avatar
Paco
Vectric Wizard
Posts: 480
Joined: Fri Sep 16, 2005 6:30 pm
Location: Valcourt, Québec, Canada
Contact:

Post by Paco »

Thanks! 8)

User avatar
Perry
Vectric Craftsman
Posts: 174
Joined: Mon Oct 24, 2005 11:06 am
Model of CNC Machine: Modified Shopbot PRT96
Location: Windsor, ON, Canada

Christmas files

Post by Perry »

Just wanted to say thanks Brian and Tony for the thoughtfulness!
Happy Holidays to you both and yours.
Perry

User avatar
Wemme
Vectric Wizard
Posts: 510
Joined: Mon Jan 30, 2006 6:31 am
Location: Christchurch, New Zealand

Post by Wemme »

Hello.
First off thanks to Tony and Co for making the trial xmas decorations.

I am trying to trial vcarve and have started with the decoration #2. xmas wreath
I have resize the material and when i click to recalculate the tool paths Vcarve has taken over
30minutes and still hasn't finished calculating paths

The material size has just been changed to 400mm x 400mm. The artwork has not been scaled just centered.
The machine is an Atholon 64 3000(2.1 Ghz) - 1GB Ram - Win XP SP2 which is a good spec machine.
Vcarve is using 100% cpu and ~325Mb of ram

Is this Typical tool path calculating time (I'm still wait for it to finish) or have I done something wrong?

Any ideas or help appreciated.
Cheers

User avatar
Tony Mac
Vectric Alumni
Posts: 1965
Joined: Sat Jul 30, 2005 6:24 pm
Location: UK
Contact:

Post by Tony Mac »

Hello Wemme,

You have identified a slight problem that will now be fixed. The parameters stored in toolpaths for this sample file are in Inches and are not being updated when swapping to Metric.

Delete the 2 toolpaths
Create new toolpaths - using the required cutters

The new toolpaths should be calculated almost instantaneously.

Sorry for any inconvenience this may have caused and Thank you for taking the time to let us know about the problem.

Regards,
Tony McKenzie

User avatar
Wemme
Vectric Wizard
Posts: 510
Joined: Mon Jan 30, 2006 6:31 am
Location: Christchurch, New Zealand

Post by Wemme »

Tony Mac wrote:Hello Wemme,
You have identified a slight problem that will now be fixed.
Delete the 2 toolpaths
Create new toolpaths - using the required cutters
Sorry for any inconvenience this may have caused and Thank you for taking the time to let us know about the problem.
Hi Tony,
No worries I'm happy to know that this is the case.
Now when I was cutting this file it took a long time to cut.
my cut file was 180MB for a shopbot which seems a wee bit excessive.
The tool does alot of shallow cuts side by side.
Being a V cutter I hoped it would plunge deeper to get the width and hence less passes would be needed
this would mean lest total time and more output.
Is that possible with this software?

Cheers

User avatar
Tony Mac
Vectric Alumni
Posts: 1965
Joined: Sat Jul 30, 2005 6:24 pm
Location: UK
Contact:

Post by Tony Mac »

Hi again,

Sounds very wrong.

Cutting the design at 400mm x 400mm into 12.7mm thick material using a 90' V-Bit 12mm diamter cutter should create an SBP toolpath file under 1Mb and the job should cut in around 15 minutes.

Attached is the job scaled to 400mm with the toolpaths included.

Let me know how you get on with this.

Regards,
Tony
Attachments
Xmas_Decoration_400mm.zip
(428.13 KiB) Downloaded 316 times

User avatar
Wemme
Vectric Wizard
Posts: 510
Joined: Mon Jan 30, 2006 6:31 am
Location: Christchurch, New Zealand

Post by Wemme »

Hi Tony,
I Must be having a bad day.
The above Fixed my calculation time and file size issue and looks good.
The end mill worked perfect and the tool data base and vector control is excellent I very much like this.

I have now cut a new part and have an issue with loss of detail in the Vcarve.
I've added some attachments of Simulated verse real world photos.
Notice in particular the berries are not quite right. it looks as if it has cut too deep.

I used a 19mm diametre 90 degree V cutter. althought the cut path was calculated for use of a 12mm cutter this shouldn't matter
as this only should become a problem with a z plung over 12mm where as the max in this project is 6mm.

The materials and machine were set to Z=0 at the top surface.

I have checked my Z Calibration and it is correct.

Any Ideas on what I am doing wrong?

Cheers
Attachments
full.jpg
Full project, Yes it was cut on an offcut and didn't quite fit :)
(54.21 KiB) Downloaded 387 times
detail.JPG
close up on cut project
(63.25 KiB) Downloaded 381 times
pc_detail.jpg
Approx same view on simulator
(65.66 KiB) Downloaded 398 times

User avatar
BrianM
Vectric Staff
Posts: 1961
Joined: Mon May 16, 2005 10:15 am
Model of CNC Machine: A few ...
Location: Alcester U.K
Contact:

Post by BrianM »

Hi Wemme,

The tool is definitely over cutting, and in these cases there are usually problems in one or more of the following areas.
  • Z setting of tool is wrong

    Tool geometry is wrong

    Material surface is not flat
In this case, I think the errors are too extreme to put down to just tool geometry errors or material flatness.

I’ve had a close look at your images, and I think it is clear that the Z depth of the tool is wrong. The image I’ve attached demonstrates my reasoning. In the area I’ve highlighted the tool should be just cutting into the surface (the toolpath is only about 0.5mm deep at that point). It is obvious from your photographs that at this point on your machine, the tool is considerably deeper than 0.5mm below the material surface and this seems to be constant over the complete job. If you haven’t scaled the toolpath in the ShopBot software, the only reason I can think of for the tool being too deep is that the tip of the tool is not set to z = 0.0 on the surface of the material.

Regards

Brian
Attachments
ToolTooDeep.jpg
Comparison of simulation and cut piece showing tool too deep.
(72.8 KiB) Downloaded 372 times

User avatar
Wemme
Vectric Wizard
Posts: 510
Joined: Mon Jan 30, 2006 6:31 am
Location: Christchurch, New Zealand

Post by Wemme »

Hello Brian.
Thank you for your comments.
I Have check what you mentioned and have found the tool geometry was wrong, I.E. was calculated for a 60 degree and was cut with a 90.
This will account for the berries not being round and also to the deeper Z movements, I have corrected this, recalculated the cut paths.
I have check and re checked Material flatness and that Z=0 at the top surface of the material, Also The shopbot is NOT scaling the cut file.
This time the cut looks good BUT it still looks like Z is over cutting or is this now correct?
Cheers
Attachments
full.JPG
(60.17 KiB) Downloaded 374 times
detailed.JPG
(57.71 KiB) Downloaded 353 times

User avatar
BrianM
Vectric Staff
Posts: 1961
Joined: Mon May 16, 2005 10:15 am
Model of CNC Machine: A few ...
Location: Alcester U.K
Contact:

Post by BrianM »

Hi Wemme,

The tool is obviously still cutting too deep. The area you have the rule on is showing a width of about 3mm, assuming you have been cutting from the file Tony posted above, that region is 1.5mm wide. With a 90 degree tool, the tool tip should only be 0.75mm deep into the material at that point, and it is obvious from the photo that the tool is substantially deeper than that.

Also, the ends of that section of the design are also square, so the toolpath comes upto the surface at the corners leaving a sharp corner, from your photographs the corners are still round indicating that the tool is still below the material surface at that point.

Another possibility is that the tool you are using does not actually come to a sharp point. Many VBit tools have a 'flat' tip on them, and if this is the case you need to tell VCarve Wizard about the true tool shape as the toolpath needs to be different if the tool does not come to a sharp point. It is difficult to tell just from the photo, but I don't think this is the case here, it looks as though you have a sharp line at the bottom of the cuts, indicating that the tool does come to a sharp point.

So again I think there is a problem with setting the z depth of the tool. To create the difference in width you show in your photo, the tool only needs to be set 0.75mm (0.030") too deep and hence cutting at 1.5mm instead of 0.75mm. A

What method are you using to set the tool z depth? Are you setting the tool depth at the approximate centre of the material you are cutting?

Generally, if you are cutting designs with small detail it is critical that the machine is both accurate and that the z height of the tools is set very precisely. If you are cutting larger pieces the level of accuracy is not as critical, but V carving does require far more accuracy then general 2d cutting.

Regards

Brian
Last edited by BrianM on Sat Feb 04, 2006 12:12 am, edited 1 time in total.

User avatar
Wemme
Vectric Wizard
Posts: 510
Joined: Mon Jan 30, 2006 6:31 am
Location: Christchurch, New Zealand

Post by Wemme »

Hello Brian,
Thank you for your help I will have a further look in to it.
I was zeroing on 0,0 not center of material.
Regards

User avatar
Wemme
Vectric Wizard
Posts: 510
Joined: Mon Jan 30, 2006 6:31 am
Location: Christchurch, New Zealand

Post by Wemme »

Heres an odd one.

Since I have purchased vcarve wizard I no longer can work with the old samples and convert them to mm nor can i set the material size if i do it crashes vcarve. however .crv files I've made have been fine. there seem to be some really large offset values and i can't change the material size setup?
anyone else run into this??

Could someone post a zip with the .esp for this project as i would like to cut some smaller ones etc.
Thanks.

Post Reply